Holes

The Holes tool is used to create any type of normalized hole on the part. This dialog box is displayed every time you drop the IPROHoles tool on the part or when you edit an existing hole.

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Description of the User Interface

At the top of the dialog there are the buttons useful to control the placement of the hole and a combo box used to select the Unit of Measure related to the parameter of the hole. At the left of the Unit of Measure combo there is a button that is used to display a list containing all the Holes existing on the selected part. This list is very useful if you need to modify several holes at once. Clicking on the button, the dialog box will be enlarged, and the list of holes placed on the part will be displayed. At this point, selecting the hole in the list, the fields of the dialog box will be updated in order to reflect the values of the selected hole. A very powerful functionality of this tool is that, if you select an hole placed on a different part, this list will be updated in order to contain all the holes placed in the new selected part.

Components

The family of hole can be selected using the two tabs. When you change the type of the hole, the dialog box is immediately updated.

You can change the type of hole clicking one of the four option buttons placed under the tabs. Every time you change the selection, the dialog box is updated in order to show you all the parameters related to the hole.

Settings

The buttons included in this box allow you to save the current hole settings. This allows them to be quickly recalled in future sessions. From the combo box you can select saved holes, while the button on the right allows you to open a dialog box for managing and reordering settings (which are separate for plain and threaded holes).

Parameters

• Type GAS - When this button is checked, a combo boxcontaining all the normalized GAS diameters becomevisible.

• Diameter - d or M - This option is used to select orto insert the required diameter for the hole. A label placed at the right of this item shows the Actual Diameter. In the case of simple hole, the Actual Diameter is the value of diameter minus the tolerance value. In the case of thread holes the Actual Diameter is the diameter minus the pitch.

  • Pitch Thread Coarse/Fine - If you select a threaded hole, this combo box allows you to select the pitch type.
  • Tolerance - If this option is selected, a combo box containing available tolerances will be displayed.

• Hole Depth - L - This option is used to insert or select the depth of the hole. This option is disabled if you check the Through option.

  • Through - If this option is selected, the hole goes through the entire part from the selected face to the opposite face.

• Bottom V - a - This option is used to control thebottom shape of the hole. This option is disabled ifyou check the Through option or the Flat option. When this option is enabled you can set the bottomangle of the hole.

• Taper Angle - g - This option is used to set a taperangle for the hole. To enable this item, you have tocheck the Apply option.

• Hole Color - This option applies a color to the inside wall of the hole.

• Chamfer End - with this option it is possible to apply a chamfer on both edges of the hole (only initial, or initial and final if it’s through)

• Drill Parts - If you select this option, you can “drill” multiple parts in one operation. In this way, you can generate holes even in the parts below the first one, up to the desired length. If, you also enable Through opt. the Drop-down menu Drill Parts will also be visible, from here you can set the number of parts to be drilled; which will generate as many through holes in the selected parts below.

When you select a Counter Sink or Counter Bore hole, the section related to these parameters becomes visible.

The items contained in this section are used to set the diameter, the depth and/or the angle of a counter bore, counter sink or counter drill hole. Furthermore two buttons allow you to automatically load the Standard values defined for the hole.

When you select a Thread hole, the section related to thread parameters becomes visible.

The items contained in this section are used to define the Pitch of the thread, the length of the thread and the callout to set in the 2D drawing.

The data structure behind Holes

All the data files related to hole are placed in the folder ..\Norme\Holes
This is the list of the files contained in the folder and a description of their structure:

Diameters.dat - Diameters_ENG.dat

These files contain the list of available diameters and their associated tolerances. Any row starting with the char # is considered as a comment. The row starting with the tag Toll is used to define the label of the Tolerance available. All the values after the Toll tag, will be inserted in the Tolerance combo box.

## ============================================================================
## * IRONPROXT - PARAMETRICLIBRARY - FronemaSrl *
## ============================================================================
##
##		Bohrungsdurchmesser / Diameters for Holes
##
<Toll> H5     H6     H7     H8     H9     H10    H11    H12    H13    H14    +1mm
##Diam H5     H6     H7     H8     H9     H10    H11    H12    H13    H14    +1mm
1.6	   0.004  0.006  0.01   0.014  0.025  0.040  0.060  0.100  0.140  0.250  1
2      0.004  0.006  0.01   0.014  0.025  0.040  0.060  0.100  0.140  0.250  1
2.5    0.004  0.006  0.01   0.014  0.025  0.040  0.060  0.100  0.140  0.250  1
3      0.005  0.008  0.012  0.018  0.030  0.048  0.075  0.120  0.180  0.300  1
3.5    0.005  0.008  0.012  0.018  0.030  0.048  0.075  0.120  0.180  0.300  1
4      0.005  0.008  0.012  0.018  0.030  0.048  0.075  0.120  0.180  0.300  1
4.5    0.005  0.008  0.012  0.018  0.030  0.048  0.075  0.120  0.180  0.300  1
...
...

The first value of the row is considered as a valid diameter. All the following values are related to the tolerance values.

CDiameters.dat - CDiameters_ENG.dat

These files contain the list of the available diameters and depths related to counter depth holes. Any row starting with the char # is considered as a comment.

## ======================================================= 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## =======================================================
##                
##  Counterbore Diameters for Holes                
##
## HoleDiam	 CBoreDiam  CBoreDepth
1            2.5        1.5	
2            4.5        2.5
3            6.0        3.5
3.5          6.0        3.5		
4            8.0        4.5
4.5          7.5        4.5
5            10.0       5.5
...
...

The first value of the row is considered a valid hole diameter. The second field is the Counter Bore diameter and the third is the Counter Bore Depth. Looking at picture you can see that if you set an hole diameter between 3 and 3.5, the CBore diameter will be set to 6 and the depth will be set to 3.5

ThreadDiameters.dat - ThreadDiameters_ENG.dat

These files contain the list of the available diameters and Pitches or Thread per Inch. Any row starting with the char # is considered as a comment.

## ======================================================= 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## =======================================================
##                
##  Thread Diameters for Holes                
##               
#Diam	Pitch1	Pitch2
2.5		0.35	0.45
3		0.35	0.5
4		0.5		0.7
5		0.5		0.8
6		0.75	1
8		1		1.25
10		1.25	1.5
12		1.25	1.75
14		1.5		2
16		1.5		2
18		1.5		2.5
20		1.5		2.5
22		1.5		2.5
...
...

The first value of the row is considered a valid hole diameter. The first field is the diameter of the hole, other fields are the standard pitch. The English definition of the file, is a little bit different. The first field is the diameter of the hole and the following are the Thread per Inches. Looking at picture you can see that for an hole diameter between 18 and 20, the Pitch1 is 1.5 and the Pitch2 is 2.5

Length.dat - Length_ENG.dat

These files contain the list of the available standard length for the holes.

GASDiameters.dat - GASThreadDiameters.dat

These files contain the standard diameter values related to GAS normative. The structure of the files are self-explaining.

CounterAngle.dat

This data file contains a list of available angle for the bottom shape of the hole

NPT Holes

The Holes-NPT Holes tool is used to create NPT Hole (National Pipe Thread) in the scene. This dialog box is displayed every time you drop the NPT Holes tool in the scene or when you edit an existing NPT hole.

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Settings

The items included in this box enable you to save the current setting of the hole. This enables you to recall them quickly in future sessions. The buttons included in this section enable you to save, remove or apply any saved setting.

Parameters

• Normative - This option is used to select the standard diameters in inches or millimeters.
• Hole Diam. - This option is used to select the required diameter for the hole.
• Hole Depth - This option is used to insert or to select the depth of the hole. With the option at right you can see the measurement in inches or millimeters.
• Taper Angle - This option shows the draft angle of the hole.
• Thread Pitch - This option shows the Thread Pitch of the hole. To enable this item, you have to check the Edit option.
• Callout - If you want assign the callout in the 2D drawing, check this option.

The data structure behind NPT Holes

All the data files related to NPT hole are placed in the folder ..\Norme\Holes\

This is the list of the files contained in the folder and a description of their structure:

NPTRules.ini - NPTDiameters.dat - NPTDiametersMM.dat

These files contain the standard diameter values (in inches and millimeters) related to NPT normative.

## ======================================================== 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## ========================================================
##
# Name   |  Data File           |Callout| 0=MM 1=Inches
NPT_IN 	 | NPTDiameters.dat		|  NPT	|  1		
NPT_MM 	 | NPTDiametersMM.dat	|  NPT	|  0

## =================================================================== 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## ===================================================================
##                
## NPT Thread Hole Diameters                 
## separator field is TAB
## Units are in inches
##          
## Insider_Diam NominalSize  Pitch1   Pitch2  Length    TaperAngle
0.337 			1/8			 0.03571  0	      0.2441 	1.79
0.451 			1/4			 0.05262  0	      0.3701 	1.79
0.589 			3/8			 0.05262  0	      0.3812 	1.79
0.734 			1/2			 0.05262  0	      0.5000 	1.79
0.950 			3/4			 0.07143  0	      0.5551 	1.79
1.193 			1			 0.07143  0	      0.6378 	1.79
1.534 			1 1/4		 0.09091  0	      0.7284 	1.79
1.766 			1 1/2		 0.09091  0	      0.7284 	1.79
...
...

## =================================================================== 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## ===================================================================
##  
## NPT Thread Hole Diameters                 
## separator field is TAB
## Units are in mmillimeters
##         
## Insider_Diam NominalSize  Pitch1   Pitch2  Length    TaperAngle
8.566           1/8          0.9071   0       6.2       1.79
11.445          1/4          1.3368   0	      9.4       1.79
14.950          3/8          1.3368   0       9.7       1.79
18.631          1/2          1.3368   0       12.7      1.79
24.117          3/4          1.8143   0       14.1      1.79
30.291          1            1.8443   0       16.2      1.79
38.952          1 1/4        2.3091   0       18.5      1.79
44.845          1 1/2        2.3091   0       18.5      1.79
...
...

The structure of the files are self-explaining.

Centre Holes

The CentreHoles tool is used to create Centre Hole on the shaft part. This dialog box is displayed every time you drop the Centre Holes tool on the part or when you edit an existing Centre hole.

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Components

You can change the type of centre hole by clicking a drop down button.

When you change the type of the hole, the dialog box updated the Norme text box.

In the status bar, it shows a warning message if the diameter of the hole is not compatible with the diameter of the shaft.

The data structure behind Centre Holes

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: CentreHoles.ini and *.uni

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• Type -> the number is related to icon of the component in the User Interface.
• Table -> Data file Name of the Standard Rule.
• Label -> Description of the Standard Rule in the User Interface.

This is the structure of a CentreHoles.ini file

# Type	|   Table           |   Label
1       |   UNI3220A.UNI    |   UNI3220-A
2       |   UNI3220B.UNI    |   UNI3220-B
3       |   UNI3220R.UNI    |   UNI3220-R

The *.uni files, contain the fields of the standard values related to hole normative; the structure of the files are self-explaining.

This is the structure of a UNI3220A.UNI file

# dInt  |   dExt    |   l       |   r       |   NotSuggested
0.50    |   1.06    |   1.10    |   0.00    |   1
0.63    |   1.32    |   1.40    |   0.00    |   1
0.80    |   1.70    |   1.70    |   0.00    |   1
1.00    |   2.12    |   2.10    |   0.00    |   0
1.25    |   2.65    |   2.60    |   0.00    |   1
1.50    |   3.35    |   3.20    |   0.00    |   0
...
...

Slot Hole

The Slot Hole tool create slot on the part.

Operativity

1. Drop the tool on the part.
2. Set parmeters.

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Fasteners

This dialog box is displayed every time you drop the Fastener tool in the scene or when you edit an existing component.

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Settings

The items included in this box enable you to save the current setting of the component. This enables you to recall them quickly in future sessions. The buttons included in this section enable you to save, remove or apply any saved setting.

Components

This section is composed by five tabs. These tabs enable you to select the type of component. Every tab contains a family of components. On the left side of this section there is a drop down button that is used to select the type of the component. Moving the cursor over the icons of the components, it’s displayed a tooltip which describes the component. As soon as a new component is selected, all the items in the dialog box will be updated in order to display the available standards and dimensions.

Create Hole… and Place on All… are better explained later.

In order to avoid this behavior you can do one of these operations:

• Disable the behavior in the IPROSettings: This is a general setting, and the hole will not be elaborated when you will move a screw; see Elaborate Automatic Holes
• Keep pressed the Shift key during the TriBall translation.
• Create a configuration. In a configuration the holes created by Fasteners are not moved. (If you want to have a configuration where the the automatic update of the holes is active start the name of the configuration with + or _ chars).

Parameters

The central section of the dialog box contains the options useful to select the standard and the dimensions of the component. These parameters are: Standard Name, Component Type, Length and Material.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component. The section is divided in two parts: BOM Information and Custom Information.

Status bar

The status bar reports the description of the selected standard rule. If you click on description Library Data Manager starts to modify the description and the rules to create the bill of materials. Close to it, on the right, there is a button that enable you to edit the geometric data file, launching the Library Data Manager - Geometry…

Create Hole Locked to Fastener

Screws and Bolts components have a drop down section that enables you to set the properties of the holes associated to the element. In fact Fasteners can automatically create and associate holes to any screws or bolts placed in the scene. These are the items and the options available in this section:

• Set Transparent - Option to make the fisrt part on which the command is dragged transparent.
• First Part - This option is used to define the parameters of the automatic hole applied to the first part. By setting the drop-down button, the type of hole can be selected. You can set a tollerance for the hole.
• Intermediate Part(s) - option to define the type of hole to be applied to all parts placed between the first and last part. It’s possible to set a tollerance for the holes.
• Last Part - option to define the type of hole to be applied to the last part that has an interference with the current fastener. You can set a tollerance for the hole.
• Set Extra Length Values - Allow you to add a length to the threaded and after thread hole.
• Look depth to Screw Length - When this option is active, the length of the first hole is the same of the length of the fastener.

Place on All Equal Holes of the Face

If there are holes on the part on which the screw is dropped, and if it drop the screw on the edge of a hole, the “Place on All Equal Holes of the Face” check box is displayed, which if activated will automatically place a screw for each hole equal to the one selected.

Placement of Associated Fasteners

The Fasteners has some useful behaviors which improve your productivity. In fact when you drop the tool over an existing component, Fasteners automatically gets the existing parameters and associate the new component to the existing one. For example, if you drop the tool on the leg of an existing M10 screw, the dialog box will propose you to place a washer or a nut related to the M10 dimension. Furthermore, if you edit the screw (or the nut), the other component will be modified according to the new selected dimension.

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If the selected dimension doesn’t exist for that component, it will be suppressed. For example if you change the dimension of the screw from M10 to M18, and the nut of M18 is not available in the data file, it is not changed but it is suppressed.

Edit of Screw or Bolt length

You can change the length of the screws (or bolts) editing the component with a double click. Anyway if you select the IShape leg of the component, you can change it dragging the handle in the desired position. Fasteners automatically elaborates the new requested length and it sets the length to the closest value in the data file. Furthermore all the BOM Information, Part Name and Custom Data are updated.

Fasteners Assembly

This command is used to place in the scene an assembly composed by a screw, washers and nut.

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Settings

The items included in this box enable you to save the current setting of the component. This enables you to recall them quickly in future sessions. The buttons included in this section enable you to save, remove or apply any saved setting.

Components

This section is composed by four tabs: Screw, Washer1, Whaser2 and Nut. Every tab is used to set the property of the related component. Every section contains a drop down button used to select the kind of component to use.

Parameters

The central section of the dialog contains all the options useful to select the standard and the dimensions of the selected component. For the Screw, these parameters are: Standard Name, Component Type, Length and Material.

For other components the options available are only Standard Name and Material.

The screw is the master component. When you select a type of screw, washers and nut are automatically set to the same type.

The check button Active is used to add or remove a washer or a nut to the assembly.

When the selected type doesn’t exist in the data file, the check button is automatically unchecked and the label “Measure not Found” is displayed.

When the Active check button is changed, the preview image is updated in in order to show you which component will be included in the assembly.

The text placed in the middle of the dialog is used to insert the distance to keep between the two washers.

If you are placing the Fastener Assembly on existing part, it’s possible to calculate this value automatically clicking on the Wizard button.

In this case IPROFasteners will calculate all the existing intersection at the length specified in the Length combo box. The names of part found will be placed in the combo box at the right of the Wizard button. When you select on the these part in the combo, the calculated value will be set in the distance item text.

Inside the tab of Screw, there is the drop down button used to set the properties of the automatic holes associated to the screw.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component for the BOM (Part BOM Info and Custom Info). When the Bolt tab is selected, it’s possible to set the BOM Information also for the assembly that contains the components.

For a detailed explanation see BOM information

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Fasteners Library

With this tool you can insert an fasteners element from your library of files into the scene.

Operativity

• Drop the tool into the scene.

In the dialog box, you can, in the first combo box, select the User Library folder that contains the element you want to insert,

then in the second combo box, select the item you want to insert.

Update Fasteners Holes

The “Update Fastener Holes” tool allows to recalculate the automatic drilling functions produced by the bolts to which they are associated; for example if a part has been inserted that must be drill, or if a bolt has been removed.

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To update the holes:

1. Select the assembly or parts to be updated
2. drag the command into the scene with the left mouse button

To delete unnecessary holes:

1. Select the assembly or parts to be updated
2. drag the command to the scene with the right button

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Seegers

The Seegers tool is used to create Seeger on the shaft part. This dialog box is displayed every time you drop the Seeger tool in the scene or when you edit one.

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The Seeger can be placed also on cylindrical parts, drop the tool on an circular edge or face and the seeger inherits the shaft dimensions.

Components

The family of seeger can be selected using the two tabs.

You can change the type of seeger clicking of the option buttons placed under the tabs.

The Set Transparent option allows you to make it transparent so that you can more easily position the component in specific situations.

Parameters

• Standard Name - Using this dialog box, the user can select the correct rule.
• Type - This combo box contains all the values related to the selected rule. When the user drags a component over on circle edge (for example, if the user drags a seeger over a shaft), a check control named Auto will be shown. Using this toggle control, it’s possible that the seeger inherits the shaft dimensions.
• Hollow Mode - This box lets you choose between the hollow mode: none, active, only hollow (in this case the seeger is not positioned). When the user activates the hollow, the check control of the Chamfer is activated to do so on the edge of the groove.
• Material - Using this combo box, the user could select the code of the material related to the component.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information.

For a detailed explanation see BOM information

Status bar

The status bar reports the description of the selected standard rule. If you click on description Library Data Manager starts to modify the description and the rules to create the bill of materials. Close to it, on the right, there is a button that enable you to edit the geometric data file, launching the Library Data Manager - Geometry…

The data structure behind Seeger

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: seeger.ini and ringN.DIN

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• DataFile -> File containing the data values useful to build the component
• Rule -> Name of the Standard Rule
• Description -> Description of the Standard Rule
• MaterialFile -> Data file containing the materials allowed for this kind of component

For example, this is the structure of a Seeger.ini file

#DataFile	Rule		Description	                	MaterialFile
[1]
471.DIN	|	DIN471	|	Elastic ring for security shaft	|	seegers.dat

[2]
472.DIN	|	DIN472	|	Elastic ring for security hole	|	seegers.dat

[3]
4VA.DIN	|	DIN4VA	|	Seeger V for shaft	|	seegers.dat

[4]
4VJ.DIN	|	DIN4VJ	|	Seeger V for hole	|	seegers.dat

[5]
983.DIN	|	DIN983	|	Seeger K per shaft	|	seegers.dat

[6]
984.DIN	|	DIN984	|	Seeger K for hole	|	seegers.dat
[End]

Under each section it is possible to place several records; every record refers to a particular rule.

The material data file contains all the materials available for the component. All the material files are stored in the folder Norme.

The ringN.DIN files, contain the fields of the standard values related to seeger normative; the structure of the files are self-explaining.

## ===================================================================================
## * IronPROLibrary Data Manager - *** Fronema Srl *** - www.ironcad.it
## ===================================================================================
## Saved On: 30/06/2019 15:13:19
##------------------------------------------------------------------------------------
#Code |  d1  | s   | a   |  d3  | d5  |  d2  | m   |  t  |  AFT |PartNumber(Optional)|  
##------------------------------------------------------------------------------------
8     |  8.0 | 0.8 | 2.4 |  8.7 | 1.0 |  8.4 | 0.9 | 0.2 |  1.0 |  
9     |  9.0 | 0.8 | 2.5 |  9.8 | 1.0 |  9.4 | 0.9 | 0.2 |  1.0 |  
9.5   |  9.5 | 1.0 | 3.0 | 10.3 | 1.2 |  9.9 | 1.1 | 0.2 |  1.0 |  
10    | 10.0 | 1.0 | 3.2 | 10.8 | 1.2 | 10.4 | 1.1 | 0.2 |  1.0 |  
10.5  | 10.5 | 1.0 | 3.2 | 11.3 | 1.2 | 10.9 | 1.1 | 0.2 |  1.0 |  
11    | 11.0 | 1.0 | 3.3 | 11.8 | 1.2 | 11.4 | 1.1 | 0.2 |  1.0 |  
12    | 12.0 | 1.0 | 3.4 | 13.0 | 1.5 | 12.5 | 1.1 | 0.25|  1.0 |  
13    | 13.0 | 1.0 | 3.6 | 14.1 | 1.5 | 13.6 | 1.1 | 0.3 |  1.0 |  
......

Orings

The Orings can be placed also on cylindrical parts, drop the tool on an circular edge or face and the Orings inherits the shaft dimensions.

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Components

The family of Orings can be selected using the two tabs.

You can change the type of Orings clicking of the option buttons placed under the tabs.

The Set Transparent option allows you to make it transparent so that you can more easily position the component in specific situations.

Parameters

• Standard Name - Using this dialog box, the user can select the correct rule.
• Type - This combo box contains all the values related to the selected rule.
• Diam. Shaft/Hole - This combo box contains all the diameter values related to the selected rule. When the user drags a component over on circle edge (for example, if the user drags a Orings over a shaft), a check control named Auto will be shown. Using this toggle control, it’s possible that the Orings inherits the shaft dimensions.
• Diam. Torus - Using this combo box, the user could select the torus diameter related to the rule.
• Hollow Mode - This box lets you choose between the hollow mode: none, active, only hollow (in this case the oring is not positioned). When the user activates the hollow, the check control of the Chamfer is activated to do so on the edge of the groove.
• Material - Using this combo box, the user could select the code of the material related to the component.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information.

For a detailed explanation see BOM information

Status bar

The status bar reports the description of the selected standard rule. If you click on description Library Data Manager starts to modify the description and the rules to create the bill of materials. Close to it, on the right, there is a button that enable you to edit the geometric data file, launching the Library Data Manager - Geometry…

The data structure behind Oring

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: ORing.ini and OringN.UNI

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• DataFile -> File containing the data values useful to build the component
• Rule -> Name of the Standard Rule
• Description -> Description of the Standard Rule
• MaterialFile -> Data file containing the materials allowed for this kind of component

For example, this is the structure of a ORing.ini file

#	Data file	Rule		Description				 Material File
[1]
ShaftDynAS.UNI	|	AS/BS	|	O-Rings dynamic seal for shaft	|	orings.dat
ShaftDynSMS.UNI	|	SMS 	|	O-Rings dynamic seal for shaft	|	orings.dat
ShaftDynM.UNI	|	Metrico	|	O-Rings dynamic seal for shaft	|	orings.dat

[2]
ShaftStaAS.UNI	|	AS/BS	|	O-Rings static seal for shaft	|	orings.dat
ShaftStaSMS.UNI	|	SMS	    |	O-Rings static seal for shaft	|	orings.dat
ShaftStaM.UNI	|	Metrico	|	O-Rings static seal for shaft	|	orings.dat

[3]
HoleDynAS.UNI	|	AS/BS	|	O-Rings dynamic seal for hole	|	orings.dat
HoleDynSMS.UNI	|	SMS	    |	O-Rings dynamic seal for hole	|	orings.dat
HoleDynM.UNI	|	Metrico	|	O-Rings dynamic seal for hole	|	orings.dat

[4]
HoleStaAS.UNI	|	AS/BS	|	O-Rings static seal for hole	|	orings.dat
...
...

Under each section it is possible to place several records; every record refers to a particular rule.

The material data file contains all the materials available for the component. All the material files are stored in the folder Norme.

The OringN.UNI files, contain the fields of the standard values related to oring normative; the structure of the files are self-explaining.

## =================================================================================
## * IronPROLibrary Data Manager - *** Fronema Srl *** - www.ironcad.it
## =================================================================================
## Saved On: 30/06/2019 18:11:00
## ---------------------------------------------------------------------------------
## CODE |   A   |   B    |   C    |  d1    | d2 (Toro) |  AFT |PartNumber(Optional)| 
## ---------------------------------------------------------------------------------
OR2007  |  2.0  |   5.2  |  2.5   |  1.78  |     1.78  |  1.0 |
OR2010  |  2.5  |   5.7  |  2.5   |  2.57  |     1.78  |  1.0 |
OR2012  |  3.0  |   6.2  |  2.5   |  2.90  |     1.78  |  1.0 |
OR2015  |  4.0  |   7.2  |  2.5   |  3.69  |     1.78  |  1.0 |
OR2018  |  4.5  |   7.7  |  2.5   |  4.48  |     1.78  |  1.0 |
OR2021  |  5.0  |   8.2  |  2.5   |  5.28  |     1.78  |  1.0 |
OR2025  |  6.0  |   9.2  |  2.5   |  6.07  |     1.78  |  1.0 |
OR106   |  7.0  |  10.2  |  2.5   |  6.75  |     1.78  |  1.0 |
OR2031  |  8.0  |  11.2  |  2.5   |  7.66  |     1.78  |  1.0 |
OR108   |  9.0  |  12.2  |  2.5   |  8.73  |     1.78  |  1.0 |
OR109   |  9.0  |  13.8  |  3.5   |  9.13  |     2.62  |  1.0 |
...
...

Holder Rings

The HolderRings can be placed also on cylindrical parts, drop the tool on an circular edge or face and the HolderRings inherits the shaft dimensions.

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Components

The family of HolderRings can be selected using the preview button.

You can change the type of HolderRings clicking of the option buttons placed under the preview.

Parameters

• Standard Name - Using this dialog box, the user can select the correct rule.
• Type - This text box contains the values related to the selected rule.
• Diam. Shaft - This combo box contains all the diameter values related to the selected rule. When the user drags a component over on circle edge (for example, if the user drags a HolderRings over a shaft), a check control named Auto will be shown. Using this toggle control, it’s possible that the HolderRings inherits the shaft dimensions.
• Diam. Ring - Using this combo box, the user could select the ring diameter related to the rule.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information. For a detailed explanation see BOM information

Status bar

The status bar reports the description of the selected standard rule. If you click on description Library Data Manager starts to modify the description and the rules to create the bill of materials. Close to it, on the right, there is a button that enable you to edit the geometric data file, launching the Library Data Manager - Geometry…

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The data structure behind HolderRings

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: ANtenuta.ini and *.UNI

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• DataFile -> File containing the data values useful to build the component
• Rule -> Name of the Standard Rule
• Description -> Description of the Standard Rule

For example, this is the structure of a ANtenuta.ini file

#	Data file       Rule			Description
[1]
S-CRW1.UNI  	|	ISO_CRW1	|	Holder rings for rotating shaft

[2]
S-HMSA27.UNI	|	ISO_HMSA27	|	Holder rings for rotating shaft with dust seal
S-HMSA7.UNI	    |	ISO_HMSA7	|	Holder rings for rotating shaft with dust seal

[3]
S-HMSA27.UNI	|	ISO_HMSA27	|	Holder rings
S-CRS1.UNI	    |	ISO_S-CRS1	|	Holder rings

[End]

Under each section it is possible to place several records; every record refers to a particular rule.

The *.UNI files, contain the fields of the standard values related to HolderRings normative; the structure of the files are self-explaining.

## =================================================================================
## * IronPROLibrary Data Manager - *** Fronema Srl *** - www.ironcad.it
## =================================================================================
## Saved On: 29/04/2019 17:13:02                                         
##-------------------------------------------------------------------
##   CODICE     | d1        | d2        | b         | AFT       |
##-------------------------------------------------------------------
CR19x37x10      |    19.0   |    37.0   |    10.0   |     1.0   |
CR20x30x5       |    20.0   |    30.0   |     5.0   |     1.0   |
CR20x30x7       |    20.0   |    30.0   |     7.0   |     1.0   |
CR20x32x7       |    20.0   |    32.0   |     7.0   |     1.0   |
CR24x38x10      |    24.0   |    38.0   |    10.0   |     1.0   |
CR26x42x8       |    26.0   |    42.0   |     8.0   |     1.0   |
CR27x37x7       |    27.0   |    37.0   |     7.0   |     1.0   |
CR30x45x8       |    30.0   |    45.0   |     8.0   |     1.0   |
...
...

Bearings

The Bearings tool is used to create Bearing on the shaft part. This dialog box is displayed every time you drop the Bearing tool in the scene or when you edit one.

The Bearing can be placed also on cylindrical parts, drop the tool on an circular edge or face and the bearing inherits the shaft dimensions.

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Components

The family of Bearing can be selected using the three tabs.

You can change the type of bearing clicking of the option buttons placed under the tabs.

At the right of the component there is a icon,

which, if clicked, it changes the state of hidden or visible of the bearing balls.

Parameters

• Standard Name - Using this dialog box, the user can select the correct rule.
• Type - This text box the values related to the selected rule.
• Diam. Int. - This box lets you choose internal diameter of bearing related to the selected rule. When the user drags a component over on circle edge (for example, if the user drags a bearing over a shaft), a check control named Auto will be shown. Using this toggle control, it’s possible that the bearing inherits the shaft dimensions.
• Diam. Ext. - Using this combobox, the user could select the external diameter of the related selected internal diameter.
• Component Type - You can select whether to create the bearing as a single Part or as an Assembly consisting of three parts.
• Lock Mode - If selected, component editing is prevented.
• Create Hole - If selected, a hole (with tolerance) will be created for the outer diameter of the bearing.
• Reverse - If selected, the hole changes direction.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in three parts:

For a detailed explanation see BOM information

Bearing Tech InfoCustom Information is specific to bearings, it’s a collection of information about the bearing. When you click on the Custom Info tab,

it is displayed a three column grid showing the information associated to the component.

Status bar

The status bar reports the description of the selected standard rule. If you click on description Library Data Manager starts to modify the description and the rules to create the bill of materials. Close to it, on the right, there is a button that enable you to edit the geometric data file, launching the Library Data Manager - Geometry…

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The data structure behind Bearing

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: bearing.ini and bearingN.uni

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• DataFile -> File containing the data values useful to build the component
• Rule -> Name of the Standard Rule
• Description -> Description of the Standard Rule

For example, this is the structure of a Bearing.ini file

#	Data file	    Rule			Description
[0 1]	# [Ball]
4259.uni	    |	UNI4259		|	Radial bearing ball with a gear
[0 2]
42591a.uni  	|	UNI42591	|	Ball bearing with gear and oblique contact
[0 3]
4259Q4C.uni	    |	UNI4259		|	Ball bearing with four conctats and a gear
...
...
[1 1]	# [Roller]
4259rNU.uni	    |	UNI4259RC	|	Radial with cilindrical roll
[1 2]
4259rNJ.uni	    |	UNI4259RC	|	Radial with cilindrical roll and a gear
[1 3]
4259rNUP.uni	|	UNI4259RC	|	Radial with cilindrical roll and a gear
...
...
[2 1]	# [Thrust]
603367A.uni	    |	UNI603367A	|	Axial bearing with sample effect
[2 2]
603367B.uni	    |	UNI603367B	|	Axial bearing with double effect
[2 3]
603367C.uni	    |	UNI603367C	|	Axial with cilindricals rolls
...
...
[End]

Under each section it is possible to place several records; every record refers to a particular rule.

The bearingN.ini files, contain the fields of the standard values related to bearing normative; the structure of the files are self-explaining.

## =================================================================================
## * IronPROLibrary Data Manager - *** Fronema Srl *** - www.ironcad.it
## =================================================================================
## Saved On: 11/07/2019 15:23:20
## --------------------------------------------------------------------------
## CODICE | d    | D     | B    | Cd    | Cs    | Vlg   | Vlo   |Nb | AFT |
## --------------------------------------------------------------------------
618/3     |  3.0 |  10.0 |  4.0 |   375 |   176 | 40000 | 48000 | 4 | 1.0 |
623       |  3.0 |  10.0 |  4.0 |   488 |   146 | 60000 | 70000 | 8 | 1.0 |
618/4     |  4.0 |   9.0 |  2.5 |   540 |   180 | 63000 | 75000 | 8 | 1.0 |
604       |  4.0 |  12.0 |  4.0 |   806 |   280 | 53000 | 63000 | 8 | 1.0 |
624       |  4.0 |  13.0 |  5.0 |   695 |   335 | 38000 | 45000 | 8 | 1.0 |
634       |  4.0 |  16.0 |  5.0 |   865 |   440 | 36000 | 43000 | 8 | 1.0 |
618/5     |  5.0 |  11.0 |  3.0 |   637 |   255 | 53000 | 63000 | 8 | 1.0 |
625       |  5.0 |  16.0 |  5.0 |   865 |   440 | 36000 | 43000 | 8 | 1.0 |
635       |  5.0 |  19.0 |  6.0 |  1290 |   695 | 32000 | 38000 | 8 | 1.0 |
618/6     |  6.0 |  13.0 |  3.5 |   884 |   345 | 48000 | 56000 | 8 | 1.0 |
626       |  6.0 |  19.0 |  6.0 |  1290 |   695 | 32000 | 38000 | 8 | 1.0 |
618/7     |  7.0 |  14.0 |  3.5 |   956 |   400 | 45000 | 53000 | 8 | 1.0 |
...
...

Steels

Steels tool allow to place steel profile in the scene 3D, with the possibility of managing different characteristics, such as choice of profile, automatic connections, final cuts, length calculation.

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Components

This section consists of three areas. The first icon is a drop-down button used to select the type of steel profile. The second icons group is used to select the cut or interlock at the end. The last icons group is use to activate the attachment points.

When editing a steel, a drop-down menu appears to choose which other steels to apply the same change to:

• Only this Steel,
• All Steels in this Assembly,
• All Steels in the Scene.
• Only Steels this Size in this Assembly
• Only Steels this Size in the Scene

Parameters

• Standard Name - Used to select the correct rule.
• Type - Contains all values related to the selected rule.
• Thickness - To select the shell thickness related to the rule (only available for some elements).
• Material - To select the material code related to the component.
• Length - In this text box you can enter the value of the length of element, the icon on the right (wand) allows to detect the size up to the first element that intersects forward. Dec. - is the drop-down menu that allows you to choose the precision for the inclusion of the measure.
• Model Type - To select profile details: Detailed, Squared (no fillets), Simplified (Squared Fill, for square and rectangular) the green arrow lets you choose how to give the feature: Only this Steel, to All Steels in this Assembly, or to All Steels in the scene.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component. The section is divided in two parts: BOM Information and Custom Information.

BOM Information section contains the same options of the other components, but there is this option more:

User Name Prefix - This check button controls the enable state of the text item placed on the right. If this button is checked, any string placed in the text item will be used as prefix of the User Name.

Part Number can also be generated using the Numbering tool

For a detailed explanation of the other items see BOM information

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Status bar

The status bar shows the description of the selected standard rule. If you click on description, Library Data Manager starts so you can edit the description and the rules to create the BOM. Next to it, on the right, is a button that allows you to edit the geometric data file, launching Library Data Manager - Geometry…

Steel Cut Settings

Steels components have a drop-down section that allows you to set the properties of the cut end to the element. Here are the items and the options available in this section:

• Start Section - This check is for activating the cut at the beginning, there are two options, the first is a menu to select the orientation of the cut in 90° steps, and the second is a text box to define the angle of inclination.
• End Section - This check is for activating the cut at the end, there are two options, the first is a menu to select the orientation of the cut at step of 90°, the second is a text box to define the angle of inclination.
• 45 degree Orientation - This check is for rotating 45° with respect to the z axis.
• Remove Any Cuts - This check allows you to remove cuts made with the Extend and Trim tools.

Steels Interlock

The interlock cut allows you to create the profile cut for join two steels. There are two button, one for start cut and other for end, and a text box for insert the cut tolerance. The interlock cut is available for only some steels (are ones shown in figure).

Only for angular steels the interlok icon has a switch to reverse the cut.

Create Attach Points

Steels components have a three buttons that allows you to set the attachment points of the steels associated to the other steels. In fact Steels can automatically create and associate start and end to any steels placed in the scene. Here are the items and the options available in this section:

• First button - align the new element with the reference.
• Second button - align alongside the head of the reference.
• Third button - align over the head of reference.

By clicking on the buttons repeatedly, the element that is being placing, will rotate with respect to the four faces in the side or in the head.

Second bt - align alongside the head	Third bt - align over the head

Placement of Associated Steels

The Steels has some useful behaviors which improve your productivity. In fact when you drop the tool over an existing steels component, Steels automatically gets the existing parameters and associate the new component to the existing one. For example, if you drop the tool on the HE 100, the dialog box will propose you the same element with same dimension. Furthermore, if you activate Create Attach Points, the new steels will be connected to the end.

Steels along a 2D or 3D path

Automatically positions Steels along a 2D or 3D path, even with the ability to offset.

Before drop the command in the scene, select a 2D profile or a 3D curve, then select Place Along Selected Path, this creates as many steels as there are lines in the path and cuts off the ends at the bisector; you can also create a single sweep by selecting the Create Sweep option.

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Edit of Steels length

You can change the length of the steels editing the component with a double click. Anyway if you select the IShape length of the component, you can change it dragging the handle in the desired position. Furthermore all the BOM Information, Part Name and Custom Data are updated.

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The data structure behind Steels

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: Profil.ini and steelname.uni or steelname.din or steelname.dat

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• DataFile -> File containing the data values useful to build the component
• Rule -> Name of the Standard Rule
• Description -> Description of the Standard Rule
• MaterialFile -> Data file containing the materials allowed for this kind of component

Normative Data

For example, this is the structure of a Profil.ini file:

#Data file	    | Rule		| Description                           | Material File

[1]
HEA.dat			| DIN1025-2	| Beam HE with large parallel forward	| steel.dat
HEB.dat			| DIN1025-3	| Beam IPBI						    	| steel.dat
HEM.dat			| DIN1025-4	| Beam IPBv							    | steel.dat
IPE.dat			| DIN1025-5	| Beam IPE							    | steel.dat

[2]
ISO_657-15.dat	| ISO657/15 | Beam IPN						    	| steel.dat

[3]
ISO_657-11.dat	| ISO657/11 | Beam UPN							    | steel.dat

[4]
ISO_657-1.dat	| ISO657-1	| Structural with the same angles and the same forward	| steel.dat
...
...

As you can see, under each section it is possible to place several records. Every record refers to a particular rule.

The material data file contains all the materials available for the component. All the material files are stored in the folder Norme.

With Library Data Manager, under Show Normative Data, you can change the description and rules for creating the BOM through a graphical interface.

The steelname.dat files, contain the fields of the standard values related to steels normative; the structure of the files are self-explaining.

Geometry Data

For example, this is the structure of a C.dat file:

##---------------------------------------------------------------------------------
#Code     |  A   |  L  | Th. Group (s) |  B  |  C  | AFT | PartNumber (Optional)  |  
##---------------------------------------------------------------------------------
6x20x20   |  20.0  |  0  |  @1  |  20.0  |  6.0  |  1  |  
7x20x30   |  20.0  |  0  |  @1  |  30.0  |  7.0  |  1  |  
10x20x40  |  20.0  |  0  |  @2  |  40.0  |  10.0 |  1  |  
7x25x25   |  25.0  |  0  |  @3  |  25.0  |  7.0  |  1  |  
10x30x30  |  30.0  |  0  |  @3  |  30.0  |  10.0 |  1  |  
10x30x40  |  30.0  |  0  |  @4  |  40.0  |  10.0 |  1  |  
15x30x40  |  30.0  |  0  |  @4  |  40.0  |  15.0 |  1  |  
10x30x50  |  30.0  |  0  |  @4  |  50.0  |  10.0 |  1  | 
...
##---------------------------------------------------------------------------------
## Thickness definition
@1  |  1.0  |  1.2  |  1.5  |  
@2  |  1.0  |  1.2  |  1.5  |  2.0  |  
@3  |  1.2  |  1.5  |  2.0  |  
@4  |  1.5  |  2.0  |  2.5  |  
...
## Round definition
#>Thickness | Ext. Round | Int. Round   
>1.0  |  0.2  |  
>1.2  |  0.5  |  
>1.5  |  0.5  |  
>2.0  |  1.0  |  
...

Through a graphical interface, Library Data Manager, under Show Geometry Data, you can change the dimensions of the profile, such as adding or removing rows, changing thickness or rounding data.

....
##
## Round definition
##
# >Thickness | Ext. Round | Int. Round
>1.0 | 0.0 | 0.0
>1.2 | 0.0 | 1.0
>1.5 | 3.0 | 0.8
>2.0 | 4.0 | 1.0
....

>ALL | xx | yy

>ALL | X2 | X0.5

>ALL | 0.0

Custom Steels

Custom Steels allows to place user profiles using the characteristics of the tool IPROSteels, such as the points of attachment and the cuts at the ends. User profiles are to be stored in the library ICMechanical.

For a detailed explanation to create a custom steels, see here.

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Components

The first drop down button that is used to select the category of custom steel profile. The second drop down button is used to select the type of steel profile.

This button allows you to select the display of steel: details, icons or tiles.

The last icons group is use to activate the attachment point (more info here).

below is a preview of the selected profile, the icon to activate the cuts at the ends (more info here) and a combo to select the profile details (if present, more info here),

the green arrow lets you choose how to give the feature: only this steel, to all those in the assembly, or to all of the scene.

Parameters

• Material - Using this combo box, the user could select the code of the material related to the component.
• Length - In this text box the user can insert the value of the length of element, the icon at right (wand) allows to detect the size until the first element that intersects forward. Dec. - is the combo box that allows you to choose the precision for the inclusion of the measure.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component. The section is divided in two parts: BOM Information and Custom Information.

BOM Information section contains the same options of the other components.

Part Number can also be generated using the Numbering tool

For a detailed explanation of the other items see BOM information

Status bar

If you click on icon Library Data Manager starts to modify the description and the rules to create the bill of materials.

Steel Cut Settings

Steels components have a drop down section that enables you to set the properties of the cut end to the element. These are the items and the options available in this section:

• Start Section - This check is used to activate the cut into start, there are two options, the first is a combo box for select the orientation of the cut at step of 90°, the second is a text box for define the angle of inclination.
• End Section - This check is used to activate the cut at the end, there are two options, the first is a combo box for select the orientation of the cut at step of 90°, the second is a text box for define the angle of inclination.

Create Attach Points

Steels components have a three buttons that enables you to set the attachment points of the steels associated to the other steels. In fact IPROSteels can automatically create and associate start and end to any steels placed in the scene. These are the items and the options available in this section:

• First button - align the new element with the reference.
• Second button - align alongside the head of the reference.
• Third button - align over the head of reference.

By clicking on the buttons repeatedly, the element that is being placing, will rotate with respect to the four faces in the side or in the head.

Second bt - align alongside the head	Third bt - align over the head

Placement of Associated Steels

The Custom Steels has some useful behaviors which improve your productivity. In fact when you drop the tool over an existing steels component, Custom Steels automatically gets the existing parameters and associate the new component to the existing one. Furthermore, if you activate Create Attach Points, the new steels will be connected to the end.

Custom Steels along a 2D or 3D path

Automatically positions Custom Steels along a 2D or 3D path, even with the ability to offset.

Before drop the command in the scene, select a 2D profile or a 3D curve, then select Place Along Selected Path, this creates as many custom steels as there are lines in the path and cuts off the ends at the bisector.

Edit of Steels length

You can change the length of the steels editing the component with a double click. Anyway if you select the IShape length of the component, you can change it dragging the handle in the desired position. Furthermore all the BOM Information, Part Name and Custom Data are updated.

How to create a custom library

In the Profiles folder (path: ..\ICMechanical\Library\Profiles) you can create a personal folder in which to save your profiles a FileName.ics file with the profile, and a FileName.jpg file with the preview image to be shown in the dialog box (if the .jpg is not present, the preview of .ics is used).

How to create a multiple profiles for choose detail

• Create two or more Intellishape into a same Part,
• in each 2d section draw the appropriate profile steel,

• the 2D cross section and Intellishape must all be in the same position,
• the center of the profile must match the origin of the 2d section,
• change the name of the Intellishape and prefix it with the symbol _ (the name given to intellishape is what shows up in the combo box),
  • Intellishape named _@Trim is a special name for will be used as cutting element in the trim functions (and is not displayed in the combo box),
• suppress all the Intellishape except the one is to be used as default.

The data structure behind Custom Steels

All components Custom Steels has behind him one data file - IPROLib_BOM.ini placed in the Profiles folder (path: ..\ICMechanical\Library\Profiles).

This file is used to manage the automatic generation of PartNumber, Description and Custom data.

As you can see, under each FolderName it is possible to place several records. Every record refers to a particular file.

You can add the name of your folder and fill in the various fields; if you do not, the data (Name, PartNumber, Description, Material) to fill in the BOM will be as set in each individual file.

Every record contains these fields:

• FolderName -> Folder containing the 3D file
• ComponentName-> Name of the Component
• PartNumber-> Code of the Component
• Description -> Description of the Component
• CustomDataFile-> DataFile containing the custom data to add for this kind of component more info
• Material -> Directly assigns the material in the CustomProfiles.dat file more info
• MaterialFile -> Material file to show in the Material ComboBOX, if not specified the CustomProfiles.dat file is loaded

You can edit this file with Library Data Manager

For example, this is the structure of a IPROLib_BOM.ini file

# Parameters used in these schema are:
#	<C>	FileName of element
#	<L>	Sizebox Length of the component
#	<N>	Folder of element
#	<M>	Material
#	<A1>	Start taper Angle for Steels
#	<A2>	Start orientation Angle for Steels
#	<O1>	End taper Angle for Steels
#	<O2>	End orientation Angle for Steels
#
# Character ";" is used as separator
#
# All other characters are left unchanged......
#
#	The <DEFAULT> record is used if the component name is not
#	defined inside the file. In other words, when you want apply
#	the same record to all the entries of a FolderName, 
#	set ComponentName as <DEFAULT>
#
# FolderName;	ComponentName;          PartNumber;		Description;      CustomDataFile;  Material;   MaterialFile
#
AluFlex Item;	<DEFAULT>;              ALU<C>x<L>;		ALUFLEX <C>x<L>;
Serie2000;		<DEFAULT>;              S2000<C>x<L>;	S2000 <C>x<L>;                                  Steel.dat
Bosch_Rexroth;	<DEFAULT>;              BOSCH<C>x<L>;	BOSCH <C>x<L>;                      DIN2440
Bosch_Rexroth;	38429035 Profil 60x60;	38429035;		Profil 60x60;
Bosch_Rexroth;	38429052 Profil 45x45;	38429052;	  	Profil 45x45;
...
...
FBV;	        Profilo30x30_1C;        P030030C1;		<C> H<L>;         CustomFBV1C.dat
FBV;	        Profilo30x30_2A;        P030030C2A;		<C> H<L>;         CustomFBV2A.dat
...
...

RailingsXT

With this command you can insert many different types of parametric railings into the scene.

Drag the command into the scene and set the options, to dimension the railing you can enter the values in the dialog.

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The dialog box is divided into several sections:

Pillars (with base and extension), handrails, horizontal, vertical, panels and exterior; in each section you can select the element to be used and manage its dimensions and options.

Library Folders

The folders of the RailingsXT library are located in ..\ICMechanical\Library\RailingsXT in these folders you can save custom elements such as handrails, horizontals, panel, pillars, etc.

In each folder are the 3D *.ics files and the corresponding *.dat (text file containing your preferred measurements).

How to customize RailingXT components

In order to adapt elements to the chosen dimensions, all the models that make up the railings must be parametric, and be saved in the respective folders of the library.

Assemblies or parts must contain these parameters:

• one named L which defines the depth
• one named W which defines the width
• one named H which defines the height
• one named S which defines the thickness

Furthermore, the position of the anchor will be used as an insertion point.

Here are some examples:

Square Round is a pillar part:

in order to adapt the size to the railing, the part element must contain these parameters:

• H - corresponds to the Height of the railing (minus W of the Handrail, if any)
• W - L - S - are use for adapt the element to the Measure of pillar

Frontal01 is an assembly with a pillar stump and base plate:

• DY - corresponds to Y Offset of the edge
• DZ - corresponds to Z Offset of the edge
• W - L - S - are use for adapt the stump to the Measure of pillar

Panel01 is an assembly with a glass panel and clips:

• MinW - corresponds to the minium size for inser panel among two pillars
• W - is use for adapt the element to the distance of two pillars
• H - is use for adapt the element to the Height of railing (minus W of the Handrail and Horizontals, if any)

In the case of this panel there are other parameters for clip positioning and sizing.

Steel Stairs

This command is used to place in the scene a steel staircase assembly consisting of steps, side elements and landing platform.

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Drag the command into the scene and set the options, to dimension the scale you can drag the handles of the preview or enter the values in the dialog.

Steel Stair Preview	Steel Stair

The dialog is divided into four sections:

Stair Geometry

In the first section, you can set the overall dimensions of the stair (or you can drag the handles in the preview).

Lateral Elements

In the second section, it is possible to select the type of the lateral elements of the staircase, the size, the placement (both, only right, only left), and the position (inside or outside of the size); with the first icon you change the Steel Type, while with the second icon you can use a custom steel (how to create custom steel)

when you choose to use custom steel profiles, the drop-down button for choosing the profile appears, a button also appears to set the size.

Step

In the third section, it is possible to select the type of stairs steps, the size, the offset with respect to the side elements and the minimum climb between the steps (or - slightly above - force the number of steps); with the info icon you can display a diagram for the correct sizing of the staircase.

Landing

The fourth section is for the setting of the landing plate, it is possible to select the type (Straight, Right, Left or Centered) and set its size.

Library Folders

The first icon at the top left of the dialog opens the dialog for setting the folders of the Steel Stairs library: in these folders it is possible to save the custom elements such as laterals, steps, landings and railings.

Custom elements

In order to adapt elements to the chosen dimensions, all the models that make up the staircase must be parametric, and be saved in the respective folders of the library.

Here are two examples of Lateral Elements:

Lateral1 is a part with a front parametric section:

in order to adapt to the size of the staircase, the lateral elements must contain these parameters:

• StairLength - corresponds to L of the stair geometry, is the length of the stair
• StairHeight - corresponds to H of the stair geometry, is the height of the stair
• Width - corresponds to W of the profile, it is the width of the Lateral Elem
• Height - corresponds to H of the profile, is the height of the Lateral Elem
• Thickness - corresponds to Th, is the thickness of the Lateral Elem
• FrontalModel - equal to 1, indicates that the parametric section is in front (and therefore it is not the section of the custom steel)

Lateral2 is a part with lateral parametric section (section of the custom steel):

in this case the parameter Length (of the profile) does not correspond to the length of the stair, but is used to calculate the hypotenuse between the Length(L) and Height(H) of the stair.

• Width - corresponds to W of the profile, it is the width of the Lateral Elem
• Height - corresponds to H of the profile, is the height of the Lateral Elem
• Thickness - corresponds to Th, is the thickness of the Lateral Elem
• C - corresponds to C, is the size of the flange of the Lateral Elem

Here are two examples of Steps:

Step03_SM is a SheetMetal part:

to be able to adapt to the size of the staircase, the steps must contain these parameters (at part or assembly level):

• Width - corresponds to W of the stair geometry, is the width of the stair
• Depth - corresponds to d of the step, it is the depth of the step
• Thickness - corresponds to th, is the thickness of the step

optional, only if there are screws

• ScrewOffset - distance of the screw from the edge of the step

Step06-S_Bolt is an Assembly of a Step with Grid (simplified) and bolts, nuts and washers:

Railings

This command is used to place in the scene a railings assembly consisting of a railing post, handrail elements, intermediate rail and kick strip.

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Drag the command into the scene and set the options, to dimension the railing you can drag the handles of the preview or enter the values in the dialog.

Railings Preview	Railings Preview on Steel Stair

The dialog is divided into four sections:

Railing Sizebox

In the first section, Railing Sizebox, you can set the dimensions of the railing (or you can drag the handles in the preview). Change the orientation placement position (for the railing post and for the kick strip).

In the Railing Post combo box, you can select the post element for start, end, and intermediate (which can be disable), the number of intermediate posts to be placed, the start and end offset, and choose the positioning mode with respect to the selected steel position (vertical or perpendicular).

Handrail

In this section you can select whether to position the handrail, from the combobox select the element and set the start and end extension.

Intermediate Rail

Section for selecting the intermediate rail from the combobox, and set the distance from the bottom.

Kick strip

Section for selecting the kick strip.

Library Folders

The first icon at the top left of the dialog opens the window for setting the folders of the Steel Stairs library: in these folders it is possible to save the custom elements such as railing, handrail, intermediate and kick strip.

Custom elements

In order to adapt elements to the chosen dimensions, all the models that make up the railings must be parametric, and be saved in the respective folders of the library.

Assemblies or parts must contain these parameters: Height - corresponds to H of the railing Angle - used to adapt the element to the angle of the staircase (if Vertical is set as Placement) Furthermore, the position of the anchor will be used as an insertion point, and in the case of tubular profiles an attachment point called Handrail must also be defined on top of element in order to position the handrails correctly.

And it is also needed two parameters must be defined in the assembly/part one named L which defines the depth and one named W which defines the width, these parameters are used to correctly position the intermediate elements and the kickstrip.

Here are some examples:

Example 1 is a part of simple railing post:

in order to adapt the size to the railing, the part element must contain these parameters:

• Height - corresponds to H of the railing
• Angle - it is use for adapt the element to the angle to the stair

Railing 40x40 is an assembly with a railing post and base plate:

Railing 42 T L is an assembly with tubolar railing post and a side plate:

In the case of a side railing post, there must be an attachment point to the base positioned in the center of the railing with the name Railing, this attachment point is used together with the parameters L and W to correctly position the intermediate elements and the kickstrip.

Railings Assemblies

This command is used to place a parametric railing assembly in the scene.

Drag the command into the scene and set the options, to dimension the railing you can enter the values in the dialog.

Railings Parameters	Railings Preview on Steel Stair

The dialog is divided into two sections:

Railing Sizebox

In this section, you can set the dimensions of the railing and change the orientation placement position (for the railing post and for the kick strip).

In the combo box, you can select the railing assembly.

Parameter grid

This table shows the parameters relating to the railing selected with the values that can be modified by the user.

Library Folders

The icon at the top left of the dialog opens the window for setting the Steel Stairs library folders: in this folder you can save the railing assembly.

Custom Assembly Railing

In order to adapt railing to the chosen dimensions, the assembly that make up the railing must be parametric, and be saved in the respective folder of the library.

The assembly must contain at least these parameters: Length - matches to L of the railing Height - matches to H of the railing Angle - used to adapt the element to the angle of the staircase (if the railing was released on a sloped side profile) and all other parameters required to properly size the railing

Here are some examples:

Tubes_lateral is an assembly with tubolar railing and a side plate:

in order to adapt the size to the railing, the assembly must contain these parameters:

• Length - matches to L of the railing
• Height - matches to H of the railing
• Angle - it is use for adapt the element to the angle to the stair

and the assembly and parts can contain other parameters:

• other params - are use for drive the railing

Set BOM Settings

With Set BOM Settings you can change the BOM settings for the whole scene, drag the tool into the scene and choose which settings you want to change.

You can change the UserName to:

• Part Number, Description
• Add a prefix to the Name or PartNumber
• Set the encoding mode to: Automatic, Set by User, PartNumber Auto code and Description by User, PartNumber by User and Description automatic.

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Operativity

1. Drag the command into the scene to change the settings for all steels.
2. Or, first select the steels whose BOM settings you want to change,
3. Then drag and drop the command into the scene.

Create Steel Cap and Tube Cap

With Create Steel Cap (and Tube Cap) you can add the cap part to the steel by dragging the tool over the chosen end of the steel (at the beginning or end).

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Profile Type

From the combobox it is possible to choose the section of the cap profile between: Equal, Sharp corners, Chamfered corners, Filled corners. And you can choose if Create Attach Points for link the cap to the steel.

Parameters

• Thickness - Select or type the thickness of the plate.
• Steel Dimension - This two textbox detect the size of the steel on which the command is drop, and you can edit it values.
• Offset - External offset value.
• Chamfer/Round - Chanfer/Round value, the text box changes according to the profile choice.

• Create Holes - If the check is active, you can enter the values of the four holes, diameter and distances.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component. The section is divided in two parts: BOM Information and Custom Information.

BOM Information section contains the same options of the other components, but there is this option more:

User Name Prefix - This check button controls the enable state of the text item placed on the right. If this button is checked, any string placed in the text item will be used as prefix of the User Name.

For a detailed explanation of the other items see BOM information

Create Steel Stiffener

With Create Steel Stiffener you can add the stiffener part to the steel, drag the command to the chosen end of the steel.

Profile Type

From the combobox it is possible to choose the section of the stiffener profile between: Equal, Sharp corners, Chamfered corners, Filled corners. And you can choose if Create Attach Points for link the stiffener to the steel.

Parameters

• Thickness - Select or type the thickness of the plate.
• Side 1/2 - The combobox on the right can be used to choose the positioning side.
• Offset Inside - Value of internal offset.
• Offset Outside - Value of external offset.
• Triangular Shape - Set the triangular profile, available only for T and L steels.
• Reinforcement - Dimensions of the reinforcement, if the length is 0 it will not be extended beyond the dimensions of the steel (and the width will have no effect), available only for H and and C steels.
• Off. O1 and 02 - Offset value of indentations, available only for H.
• Chanfer/Round - Chanfer/Round value, the text box on the right changes according to the profile choice.

• Create Holes - If the check is active, you can enter the values of the four holes, diameter and distances.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component. The section is divided in two parts: BOM Information and Custom Information.

BOM Information section contains the same options of the other components, but there is this option more:

User Name Prefix - This check button controls the enable state of the text item placed on the right. If this button is checked, any string placed in the text item will be used as prefix of the User Name.

For a detailed explanation of the other items see BOM information

Extend Steels

With the Extend Steels command, you can extend (or cut) two steels with each other or to a face.

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Operativity

1. Drag and Drop the command in the scene,
2. Select the first Steel,
3. Select the second steel to extend, (or Select the face to use as reference, and confirm)
4. Select the type of join between the two steels,
5. Confirm your choice.

Trim at intersection

With the Trim at intersection command, it is possible to trim the selection of steels with two or more steels at their intersection.

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Operativity

1. Select one or more Steels what you want cut,
2. Drag and Drop the command into the scene.

Trim Steels

With the Trim Steels command, you can trim (or extend) one or more steels with one or two steels as a reference for the cut.

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Operativity

1. Drag and Drop the command into the scene,
2. Select one or two Steels to use as trim references,
3. Select one or more steels to trim,
4. Confirm your choice.

You can also define a start and end tolerance for the trim and if you want any connected steels to be disconnected.

3 Corner Miter

The 3 Corner Miter tool enables users to cut three steel beams at their intersection.

Operativity

1. First select the three steels you want to cut,
2. Then Drag and Drop the command into the scene.

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Quick Trim

Quick trim allows you to cut or extend selected steels to the first intersection (in both directions).

Operativity (single steel)

1. Drag and drop the tool onto the steel you want to cut.

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Operativity (multi steels)

1. First select the steels you want to cut,
2. Then Drag and Drop the tool into the scene.

Cut Steels

With the Cut Steel command, you can cut steel into two parts by entering the distance (and possibly the offset before and after cut) from the beginning (or using TriBall) or you can cut multiple steels together.

Operativity (single cut)

1. Drag and Drop the command onto steel,
2. Insert distance, or placing triball and drag,
3. Confirm your choice.

Operativity (multi cuts)

1. Drag the command into the scene with the right mouse button,
2. Select one or two Steels to use as cutting references,
3. Select one or more steels to be cut,
4. Confirm your choice.

Detach Steels

Disconnect steels that are connected to each other with attachment points.

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Operativity (single steel)

1. Drag and Drop the command onto steel.

Operativity (multi steels)

1. Select steels,
2. Drag and Drop the command into the scene.

Connect Closed Steels

Connect the steels that had been disconnected with their attachment points (if any).

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Operativity

1. Select steels that you want connect,
2. Set the infuence area to search attachment points,
3. Drag and Drop the command into the scene.

Remove End Cuts

This tool removes cuts from steels.

(Cuts created with: Quick Trim, Trim Steels, Trim at intersection, Extend Steels, 3 Corner Miter).

Operativity

1. First select the steels you want to remove cuts,
2. Then Drag and Drop the command into the scene.

Splined Shaft

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Parameters

• Normative - Combo for select the rule.
• Material - Using this combo box, the user could select the code of the material related to the component.
• Shaft Diameter - Combo for select the internal diameter.
• Ext. Diameter - Text box for insert the internal diameter (only for Splined Hub).
• Length - Text box for insert the length.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information. For a detailed explanation see here BOM information

The data structure behind Splined Shaft

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: SplinedShaft.ini and UNIxxxx.dat

For example, this is the structure of a SplinedShaft.ini file

#
#  Name	    |FileTable       | Description      	       | CodeConf                      | Descr                                       | Material
UNI 8953 SL | UNI8953sl.dat  | Splined shaft LIGHT Series  | Splined SL <N>x<Dmin>x<Dmax>  | Splined Shaft UNI 8953 SL <N>x<Dmin>x<Dmax> | Steel.dat
UNI 8953 SM | UNI8953sm.dat  | Splined shaft MEDIUM series | Splined SM <N>x<Dmin>x<Dmax>  | Splined Shaft UNI 8953 SM <N>x<Dmin>x<Dmax> | Steel.dat
UNI 8953 HSL| UNI8953Hsl.dat | Splined hub LIGHT Series    | Splined HSL <N>x<Dmin>x<Dmax> | Splined hub UNI 8953 SL <N>x<Dmin>x<Dmax>   | Steel.dat
UNI 8953 HSM| UNI8953Hsm.dat | Splined hub MEDIUM series   | Splined HSM <N>x<Dmin>x<Dmax> | Splined hub UNI 8953 SM <N>x<Dmin>x<Dmax>   | Steel.dat

The UNIxxxx.dat files, contain the fields of the standard values related to Splined Shaft normative; the structure of the files are self-explaining.

## ========================================== 
## * Fronema Srl  -  PARAMETRIC LIBRARY
## ==========================================
##
##  Cylindrical grooves parallel sides internal centering - LIGHT Series
##
##  Order	Name  Description
##		0	DMin -> Minimum diameter shaft
##		1	DMax -> Maximum diameter shaft
##		2	B    -> L dente
##		3	N    -> N denti
##      4   DEex -> External diameter splined hub
##
<UNIT> MM
#
# DMin | DMax | B  | N  | DExt
23     | 26   | 6  | 6  | 0
26     | 30   | 6  | 6  | 0
28     | 32   | 7  | 6  | 0
32     | 36   | 6  | 8  | 0
36     | 40   | 7  | 8  | 0
42     | 46   | 8  | 8  | 0
...

Gears

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The Gears tool is used to create Spur, Rack, Bevel, Sprocket or Pulley in the scene or when you edit an existing component.

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Components

The family of gears can be selected using the tabs.

You can change the type of gears clicking of the option buttons placed under the preview.

Parameters

• Transmission Rate - This text box is available when drop spur on an existing one and use it for define rate.
• Modulus - This combo box contains all the values related to the modulus available.
• Teeth - This box lets you choose the number of teeth.
• Material - Using this combo box, the user could select the code of the material related to the component.
• Fast Mode - Select this check for positioning an schematic component.
• Authored Mode - Select this check to deny acces to intellishape.

BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information. For a detailed explanation see here BOM information

The data structure behind Gears

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: Main_NAME of Comp.ini and TableNAME.uni

Every record contains these fields:

• TableName-> File containing the data values useful to build the component
• Description -> Description of the Standard Rule
• MaterialFile -> Default materials allowed for this kind of component
• CodConf -> Configuration of Code
• and other Fields specific for each components

For example, this is the structure of a Main_Spurs.ini file

#TableName	 | Description                      | Material      | CodeConf	| Density
tb_Spur1.uni | Ruote dentate cil. mozzo laterale| C 45 UNI 7845	| RDM<Z><M>	| 7.88
tb_Spur2.uni | Ruote dentate cil.			    | C 40 UNI 7845	| RD<Z><M>	| 7.88
tb_Spur3.uni | Ruote dentate cil. in ghisa		| G 20 UNI 5007	| RDG<Z><M>	| 7.0

Under each section it is possible to place several records; every record refers to a particular rule.

The TableNAME.uni files, contain the fields of the standard values related to gears normative; the structure of the files are self-explaining.

#M	 |  Z	| D1	| DM	| B     | A
1.00 |  12	| 0.00	| 9.00	| 15.00	| 25.00
1.00 |  13	| 0.00	| 10.00	| 15.00	| 25.00
....
1.50 |  28	| 12.00	| 30.00	| 17.00	| 30.00
1.50 |  29	| 12.00	| 30.00	| 17.00	| 30.00
....
....
6.00 |  24	| 0.00	| 110.0 | 60.00	| 80.00
6.00 |  25	| 0.00	| 110.0 | 60.00	| 80.00

Place Belt

The Place Belt tool is used to place automatically belt around a selection of pulley.

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Operativity

1. Drag and Drop the command into the scene,
2. Select two or more Pulley to use as references,
3. Optional, Set BOM information,
4. Confirm your choice.

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BOM Information

The bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information. For a detailed explanation see here BOM information

The data structure behind Belt

All the data files related to belt are placed in the folder ..\Norme\Gears\Belts\Pulleys

This is the list of the files contained in the folder and a description of their structure:

• Belt_AT.dat
• Belt_GT.dat
• Belt_HTD.dat
• Belt_T.dat

These files contain the standard values related to Belt normative.

es. This is Belt_T.dat

## ========================================== 
## * Fronema Srl  -  PARAMETRIC LIBRARY
## ==========================================
##
##-------------------------------------------------------------------
#P  | Wid | Thic | Code | Description                       | Coding
2.5 | 6   | 0.6  | T2.5 | Cinghia dentata Passo metrico "T" | <W> <C>-<L>
5   | 10  | 1    | T5   | Cinghia dentata Passo metrico "T" | <W> <C>-<L>
....

The structure of the files are self-explaining.

Springs

The Springs tool is used to create Springs in the scene or when you edit an existing component.

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Components

The family of Springs can be selected using the tabs.

Parameters

• Type - This combobox let you set normal or endless Springs.
• Wire Diam. - This combo box contains all the values related to the wire diameter available.
• Coil Diam. - This box lets you choose the coil diameter.
• Sizebox - These two text boxes are used to define the two diameters, internal and external
• Pich - With this combobox you select the pitch
• Unstressed length - Length of spring unstressed, with the two tab upper the parameters let you change the state of the spring and you can select the compressed mode in this case, the label becomes purple to indicate the status changed (and the spring will be colored red)
  Note

  These are the parameters of the Compression Spring, the Extension and Torsion Springs differ in some parameters.

• Material - Using this combo box, the user could select the code of the material related to the component.
• Fast Mode - Select this check for positioning an schematic spring without wire.
• Lock Mode - Check to deny acces to intellishape.
• Show Ax - If selected, a small cylinder will be created to identify the axis of the spring.
• Use ACIS - Select this check to use the ACIS kernel instead of PARASOLID as the modeling engine.

BOM Information

Spring BOMThe bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information. For a detailed explanation see here BOM information

The data structure behind Springs

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: BOMConfig.ini and TypeOfSpring.dat

BOMConfig.ini file, contain the data values useful to build the Code

1	| Compression spring	| CS<dw>x<D>x<L0> - <R>
2	| Extension spring      | ES<dw>x<D>x<L0> - <R>
3	| Torsion spring	    | RS<dw>x<D>x<A> - <R>

TypeOfSpring.dat file, contain the data values useful to build the component

#	dw	->	Wire Diameter
#	D	->	Coil Diameter
#	s	->	Pitch
#	L0	->	Height Uncompressed
#	Ln	-> 	Height Compressed
#
#dw		|		D	|	s		|	L0		|	Ln
0.20	|	2.90	|	1.00	|	7.50	|	2.48
0.20	|	2.50	|	1.40	|	8.20	|	2.07
0.25	|	3.20	|	1.81	|	10.60	|	2.61
0.50	|	11.00	|	4.00	|	14.50	|	4.20
0.50	|	6.00	|	2.76	|	35.00	|	9.22
0.50	|	5.50	|	1.74	|	6.60	|	3.24
....

Shaft Key

The ShaftKeys tool is used to create ShaftKey on the shaft part. This dialog box is displayed every time you drop the ShaftKey tool in the scene or when you edit one.

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The ShaftKey can be placed also on cylindrical parts, drop the tool on an circular edge or face and the ShaftKey inherits the shaft dimensions.

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Components

You can change the type of ShaftKeys clicking of the combo box Normative placed into parameters.

Parameters

• Unit - This box lets you choose the measure unit.
• Normative - Using this combo box, the user can select the correct rule.
• Hollow Mode - This box lets you choose between the hollow mode: none, active, only hollow (in this case the ShaftKey is not positioned). When the user activates the hollow, the check control of the Chamfer is activated to do so on the edge of the groove.
• Material - Using this combo box, the user could select the code of the material related to the component.
• Shaft Diam. - This combo box contains all the values related to the selected rule. When the user drags a component over on circle edge (for example, if the user drags a ShaftKey over a shaft) the ShaftKey inherits the shaft dimensions.
• other Fields specific for each components

BOM Information

ShaftKey BOMThe bottom section of the dialog contains the items useful to set the information related to the component.

The section is divided in two parts: BOM Information and Custom Information. For a detailed explanation see here BOM information

The data structure behind ShaftKey

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: ShaftKey.ini and FileName.dat

Every numbered section is related to an icon of the component in the User Interface, and every record contains these fields:

• Name -> Component name that appears in the combo
• FileTable -> File containing the data values useful to build the component
• TypeKey -> Type of ShaftKey
• Description -> Description of the Standard Rule
• CodeConf -> Configuration of Code
• Descr -> Configuration of the Description
• MaterialFile -> Data file containing the materials allowed for this kind of component

For example, this is the structure of a ShaftKey.ini file

#
#  Name	   |FileTable	   |TypeKey| Description			 | CodeConf		  |	Descr 		  |	Material
#
DIN 6885 A | DIN6885A.dat  |  0    | Parallel Key Low Type	 | <b>x<h>x<l><T> |	KK<b>x<h>x<l> |	Steel.dat
DIN 6885 B | DIN6885B.dat  |  1    | Parallel Key Hight Type | <b>x<h>x<l><T> |	KR<b>x<h>x<l> |	Steel.dat
DIN 6887   | DIN6887.dat   |  2    | Taper key with gib head | <b>x<h>x<l><T> |	KR<b>x<h>x<l> |	Steel.dat
DIN 6888-1 | DIN6888-1.dat |  3    | Woodruff key		     | <b>x<h>x<l><T> |	KR<b>x<h>x<l> |	Steel.dat
DIN 6888-2 | DIN6888-2.dat |  3    | Woodruff key		     | <b>x<h>x<l><T> |	KR<b>x<h>x<l> |	Steel.dat

Under each section it is possible to place several records; every record refers to a particular rule.

The material data file contains all the materials available for the component. All the material files are stored in the folder Norme.

The FileName.dat files, contain the fields of the standard values related to ShaftKey normative; the structure of the files are self-explaining.

#
# DMin   DMax	b	   	h	   	l		t1	
#
6	|	8	|	2	|	2	|	6	|	1.2
6	|	8	|	2	|	2	|	8	|	1.2
6	|	8	|	2	|	2	|	10	|	1.2
6	|	8	|	2	|	2	|	12	|	1.2
6	|	8	|	2	|	2	|	14	|	1.2
6	|	8	|	2	|	2	|	16	|	1.2
6	|	8	|	2	|	2	|	18	|	1.2
...
...

Grooves

The Grooves tool is used to create grooves or chamfers on the shaft part.

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This dialog box is displayed every time you drop the Grooves tool on the part or when you edit (the Intellishape) an existing one.

1. Edge selected for Chamfer
2. Edge selected for Groove Grooves can be placed only on cylindrical parts, drop the tool on an circular edge (otherwise you will be shown a warning message).

Components

You can change the type of Grooves by clicking a drop down button Normative and Type.

Parameters

When you change the type of the Grooves, the dialog box updated the values text box.

In this box, it shows a warning message if the Groove is not compatible with the diameter of the shaft.

The data structure behind Grooves

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: Grooves.ini and *.dat

Every record contains these fields:

• ID -> the number is related to the component in the User Interface
• StandardName -> Component name that appears in the combo Normative
• Table -> File containing the data values useful to build the component
• FormName -> Name that appears in the combo Type
• FormType -> Type of Groove This is the structure of a Grooves.ini file

#ID	| StandardName | Table		    |FormName|   FormType
#
1	|	UNI 4386   | Form_E_UNI.dat	|	E	 |	1
2	|	UNI 4386   | Form_F_UNI.dat	|	F	 |	2
3	|	DIN 509	   | Form_E_DIN.dat	|	E	 |	1
4	|	DIN 509	   | Form_F_DIN.dat	|	F	 |	2
5	|	DIN 509	   | Form_G_DIN.dat	|	G	 |	3
6	|	DIN 509	   | Form_H_DIN.dat	|	H	 |	4
7	|	DIN 76-1   | Form_A_DIN.dat	|	A	 |	5
8	|	DIN 76-1   | Form_B_DIN.dat	|	B	 |	5

The *.dat files, contain the fields of the standard values related to Groove normative; the structure of the files are self-explaining.

#
#DMin|	DMax     |	r	 |	t	 |	b	 |  c	 |	t1	 |  a
#
0	 |	1.6		 |	0.1	 |	0.1	 |	0.5	 |	0.8	 |	0.1	 |	0
1.6	 |	3		 |	0.2	 |	0.1	 |	1	 |	0.9	 |	0.1	 |	0
3	 |	10		 |	0.4	 |	0.2	 |	2	 |	1.1	 |	0.1	 |	0
10	 |	18		 |	0.6	 |	0.2	 |	2	 |	1.4	 |	0.1	 |	0.2
18	 |	50		 |	1	 |	0.2	 |	2.5	 |	1.8	 |	0.1	 |	0.8
50	 |	80		 |	1.6	 |	0.3	 |	4	 |	3.1	 |	0.2	 |	1.1
80	 |	125		 |	2.5	 |	0.4	 |	5	 |	4.8	 |	0.3	 |	1.9
125	 |	9999999	 |	4	 |	0.5	 |	7	 |	6.4	 |	0.3	 |	4

Boss Thread1

The BossThread 1 tool is used to Boss Thread whit run-out and cylinder on the shaft part. This dialog box is displayed every time you drop the BossThread 1 tool on the part or when you edit an existing BossThread.

The BossThread 1 can be placed only on cylindrical parts, drop the tool on an circular edge or face (otherwise you will be shown a warning message).

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Settings

The items included in this box enable you to save the current setting of the BossThread. This enables you to recall them quickly in future sessions. The buttons included in this section enable you to save, remove or apply any saved setting.

Components

You can change the type of Boss Thread 1 by clicking a drop down button Normative (currently no standard is available, values must be entered by hand).

Parameters

• Diameter - This option is used to select the required diameter for the Boss Thread.
• Length - This option is used to insert or to select the length of the Boss Thread.

• Diameter - This option is used to select the required diameter for the Run-Out.
• Length - This option is used to insert or to select the length of the Run-Out.

• Diameter - This option is used to insert the required diameter for the base Cylinder.
• Length - This option is used to insert or to select the length of the base Cylinder.

• Pitch - This option shows the Thread Pitch of the BossThread. To enable this item, you have to check the Edit option.
• Chamfer - This combo let you select if you want create a chamfer at top of bossthread.
• Thread Mode - This combo let you select at right or left for the thread.
• Callout - If you want assign the callout in the 2D drawing, check this option.

The data structure behind BossThread

The BossThread 1 command is completely manual, so all diameters and lengths must be entered manually, only the pitch is driven by the file Pitch.dat (file containing the values of the available pitch) that is in the folder ../Norme/BossTherad/.

Boss Thread

The BossThread tool is used to Boss Thread on the shaft part. This dialog box is displayed every time you drop the BossThread tool on the part or when you edit an existing BossThread.

The BossThread can be placed only on cylindrical parts, drop the tool on an circular edge or face (otherwise you will be shown a warning message).

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Settings

The items included in this box enable you to save the current setting of the BossThread. This enables you to recall them quickly in future sessions. The buttons included in this section enable you to save, remove or apply any saved setting.

Components

You can change the type of Boss Thread by clicking a drop down button Normative (Standard, GAS, NPT mm and inch).

Parameters

When you change the type of the Boss Thread, the dialog box updated the value text box.

• Diameter - This label shows the measured diameter shaft, if you check the box Man., you can change it. In other cases is used to select the required diameter for the Boss Thread.
• Total Length - This option is used to insert or to select the length of the Boss Thread (including the length of the run-out). With the option at right you can see the measurement in inches or millimeters.
• Taper Angle - This option shows the draft angle of the BossThread.

• Create Run-Out - If checked let you create an run-out.
• Diameter - This option is used to select the required diameter for the Run-Out.
• Length - This option is used to insert or to select the length of the Run-Out.

• Pitch - This option shows the Thread Pitch of the BossThread. To enable this item, you have to check the Edit option.
• Chamfer - This combo let you select if you want create a chamfer at top of bossthread.
• Thread Mode - This combo let you select at right or left for the thread.
• Callout - If you want assign the callout in the 2D drawing, check this option.

The data structure behind BossThread

Every component defined in the User Interface has behind him some data files which contain properties and parameters related to the component itself. These files are placed in the folder of the standard rule. The main files associated to the family of components are the followings: BossThread.ini and *.dat

Every record contains these fields:

• Name -> Component name that appears in the combo Normative
• DataFile -> File containing the data values useful to build the component
• Callout -> Prefix to be assigned to the callout
• 0=MM 1=Inches -> unit of measure
• RunOutFile -> File containing the data values useful to build the runout

This is the structure of a BossThread.ini

## ============================================================================ 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## ============================================================================
#
# Name   |  Data File               |Callout| 0=MM 1=Inches	|  RunOutFile
Standard | ThreadDiameters.dat		|  M	|  0	    	|  RunOut.dat	
GAS      | GASThreadDiameters.dat	|  G	|  0	    	|
NPT_IN 	 | NPTDiameters.dat		    |  NPT	|  1	    	|
NPT_MM 	 | NPTDiametersMM.dat		|  NPT	|  0	    	|

The *.dat files, contain the fields of the standard values related to Boss Thread normative; the structure of the files are self-explaining.

This is the structure of a NPTDiameters.dat

## ============================================================================ 
## * IRONPROXT -  PARAMETRIC LIBRARY  -  Fronema Srl *
## ============================================================================
##
## NPT Thread Diameters                 
## 
## separator field is TAB
## Units are in inches
##          
## Outsider_Diam  NominalSize 	Pitch1	Pitch2   Length    Taper Angle
0.383 				1/8			0.03571 	0	0.15630 	1.79
0.518 				1/4			0.05262 	0	0.23661 	1.79
0.656 				3/8			0.05262 	0	0.25000 	1.79
0.825 				1/2			0.05262 	0	0.32126 	1.79
1.041 				3/4			0.07143 	0	0.37520 	1.79
...
...

Kernel Manager

Dragging this command in the scene, we can change the modeling kernel of all parts in the scene, or alternatively only selected.

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To change the kernel of all parts, select the item father (“Parasolid Parts” or “ACIS Parts”) and then click on the arrow above the list:

Violet Arrow -> changes from Parasolid to ACIS,

Blue Arrow <- change by ACIS to Parasolid.

To change the kernel only some parts, simply select it from the list and then click on the arrow to change the kernel.

With the buttons below parts lists, you can perform some operations:

• Suppress the selected parts
• Remove the suppression of selected parts
• Suppress all unselected parts
• Highlight the selected parts

External Link Manager

The External Links Manager gives you the full control over all linked files in a scene.

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The command has to be dragged to an empty area of the scene.

In dialog box there are three buttons with which you can either unlink a specified part or unlink all files in the entire scene (also with the possibility of unlink the children parts), or save with the name all parts.

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The other four buttons allow you to: save the selected link file to another location (or rename the linked file), exchange the link with another file, open the linked file, save the selected part. These buttons are enabled only if you select an item in the tree view.

In the bottom of the dialog, we have three tab to view the parts, those Linked and Not Linked

Also on the Not Linked tab is a tree view for selecting parts you want to save externally, there are also two controls: one for choosing whether to save all files in a single folder, and the other whether you want the exported part to be moved (based on the element’s own anchor) to the origin of the new file.

The Element Selection menu is useful for quickly selecting elements (Select All, Select Assemblies, Select Parts, Select Sheet Metal Parts, Delete Selection) to export externally. It also contains an option to exclude IPROFasteners and an option to manage the Linked Mirrored elements, with the option of not Selecting or Unlinking them.

While the icons above the grid are respectively for:

• Fill the grid, to set by rules all new part names, part numbers and file names
• Search and Replace text, to rename in bulk: part name, part number, file name and folder.

And the tab Linked Files with a list of all files linked.

In the tab Linked, the command Save all to New File, open a new dialog where you can manage the save of the linked parts, setting the new name and new part number, the destination folder and the file name.

This data can be changed individually for each part/assembly, selecting the relative cell within the grid and entering the new data, or by adjusting the controls placed on the top of the window you can automate some procedures.

Furthermore, if the source folder contains the 2D files of relating to linked parts, you can copy and update the links to the new file and the new folder.

All these options affect the behavior of the below grid:

• Export All Files in the Same Folder: When this option is active, the value inserted in the “New Path” column, will be copied for all the rows in the grid

• Set FileName Equal to UserName: When this option is active, the value inserted in the “New Name” column, will be copied in the “New File Name” column. In other words the exported file will have the FileName equal to the UserName of the element.

• Set FileName Equal to PartNumber: When this option is active, the value inserted in the “New PartNumber” column, will be copied in the “New File Name” column. In other words the exported file will have the FileName equal to the PartNumber of the element.

• Set UserName Equal to PartNumber: When this option is active, the value inserted in “New PartNumber”, will be copied in the “New Name” column.

• Keep the Same FileName for Identical Links: When this option is active, the value inserted in the “New Path” or “New FileName” columns, will be automatical copied in all the rows related to the links of the element. In other words, all the linked element will have the same folder and the same filename set automatically.

• Keep the Same Data for Identical Links: When this option is active, any change in the “New PartNumber” and “New Name”, will be automatically copied to all the linked elements

• Save also current Scene: When this option is active, also the main opened model will be inserted in the grid, and it will be possible to set any fields related to save options.

• Copy 2D files: This option does not affect the behavior of the grid. When this option is enabled, all ICD, EXB, and DWG files (whose filename is the same as the filename of the ICS file) in the source folder will be copied to the destination folder.

• Reassociate 2D linked files: This option doesn’t affect the behavior of the grid. When this option is active, at the end of the save/copy process, the reassociation process between 3D files and ICS files will be executed. This process runs automatically IronCAD in background and open, modify and save all the .icd files in the destination folder.

  Caution

  This process can require several time to be completed!

  Furthermore, any error or prompt for “Corrupted Styles” fill put in pause the process, waiting the input from the user.

• Copy All Other Files in Scene Folder: This option doesn’t affect the behavior of the grid. This option is active when is set the “Save Also current Scene” option. When this option is active, all the files (e.g. Pdf, Word, Excel, DXF) in the source folder, will be copied to the destination folder.

Also, with the Search and Replace button you can rename in bulk: New PartName, New PartNumber, New FileName and New Folder.

Isolate Elements

The Isolate Elements tool manages the visibility of the elements of your project. It works in two modes, for StatusColor/Category or via dialog.

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Operativity

• with the left mouse button:
  • Drag in the scene with the left mouse button, the dialog box opens to select the elements according to the StatusColor or Category.

• Dialog box, with the right mouse button:
  • Drag in the scene with the right mouse button, opens the dialog box to manage the saved states (or the interactive stored states).
  • Here you can add, rename or remove states; add or remove items from a saved state, save or update camera orientation.
  • To activate a status double-click on the name.

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Ghost Manager

The Ghost Manager tool manages the visibility of the elements of your project. It works in two modes, for StatusColor/Category or via dialogue.

Operativity

• with the left mouse button:
  • Drag in the scene with the left mouse button, the dialog box opens to select the elements according to the StatusColor or Category.

• with the right mouse button:
  • Drag in the scene with the right mouse button, opens the dialog box to manage the ghost saved states (or the interactive stored states).
  • Here you can add, rename or remove ghost states; add or remove items from a saved state, save or update camera orientation.
  • To activate a ghost status double-click on the name.

Find Suppressions

Dragging the command in the scene, a window appears with a list of parts/assemblies suppressed in the active scene, useful for finding all suppressed parts in a large assembly.

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The buttons at the top of the dialog, allow to:

• highlight the selected items in the scene,
• unsuppress the selected items,
• suppress the selected items,
• delete the selected items.

Fix Anchors

This tool allows you to reset all of the anchors of elements of the scene (or active selection) in fixed mode (disallow drag). If you want to fix also the anchors of intellishapes, drag the command in the scene with the right mouse button.

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Text 3D

This tool can create a 3D text part or 2D profile with all fonts avaible in the system.

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If you drag on an existing part, you can also choose to create a cutting or extrusion, and you can get value to write the text from: PartNumber, Description, CustomData or Parameters.

On the left side of the dialog box there are buttons to choose font, size and styles; below them is the area where you write text.

While in the right part of the dialogue there are two zones, the first to define the Shape (part, intellishape or 2d profile), if you want to create a shape for each letter, whether to use the BSpline for the curves and the level of facet; the second to define the SizeBox of the text, the aspect lock and the alignment for the multiline.

For edit the text and values, right clic on intellishape and select Add-on Properties…

This is an example of the features available.

Get Coordinates

Get coordinates, returns the coordinates of the points selected in the scene.

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Drag each time the command to the desired point, the window will be increased the list of selected points.

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In the top of the dialog are icons for:

• delete a line
• export the list to Excel
• export the list to DXF file
• display global coordinates
• display local coordinates
• display coordinate from the anchor of the element
• display an arrow pointing to the selected point

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ProDrill

PRODrill tool, get every IntelliShapes named Drill (e.g. HWDrill, DrillHERE…), and it use it to “drill” every parts that has an interference with the HWDrill IntelliShape.

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Operativity

• Drop the tool into the scene to apply the drill cuts for all parts.
• Select the assembly first, then release the tool into the scene to apply drill cuts only to the parts in the assembly.

ProDrill Naming Rules

1. Part whose names starts or end with _ are not drilled.
2. HWDrill element that contains the char + drills also element described at point 1.
3. HWDrill that contains #1 in the name, drills only elements that are in the same assembly.
4. HWDrill that contains #2 in the name, drills only element that are in different assembly.
5. HWDrill whose name start with @ , don’t drill.
6. HWDrill whose name start with # or contain _NS_ , drills elements and remain visible itself.

Visibility ProDrill

This tool shows/hides all ProDrill features in all parts of the scene.

Operativity

• Drop it in the scene with the left button to show all the HWDrill.
• Drop it in the scene with the right button to hide all the HWDrill.

Remove Drill Holes

This tool removes all features of Drill holes in all parts of the scene, drop it into the scene to run it.

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Suppress Manager

The SuppressManager tool allows you to Suppress (Unsuppress, Select and Delete) Parts, Hole and IntelliShapes based on various criteria such as Status Color, Category,Dimensions, Weight, Volume and Color. Also the tool, allows you to create Configurations from the selection results.

Drag the command to the scene to activate, the dialog is divided into five tabs:

By Status Color

Search parts based on the Status Color,

It allows you to create a Configuration from the result of the selection.

By Category

Search parts based on the Category,

It allows you to create a Configuration from the result of the selection.

Parts

Search parts based on the size (or Based equivalent Volume), you can click on the cube with the arrows to detect the dimensions of the part selected in the scene.

It allows to:

• Suppress (Unsuppress, Select or Delete) smaller or larger parts of the stated values.
• Suppress or Unsuppress the Fasteners.
• Suppress or Unsuppress the Holes.
• Create a Configuration from the result of the selection.

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Weight

Search parts based on a weight range. It allows to Suppress (Unsuppress, Select or Delete) parts included or not included of the stated values.

It allows you to create a Configuration from the result of the selection.

Holes

Search holes (and the H IntelliShapes) based on the size (or Based equivalent Volume), you can click on the cube with the arrows to detect the dimensions of the part selected in the scene. It allows to Suppress (Unsuppress, Select or Delete) smaller or larger holes of the stated values. It allows you to Suppress All Holes. It allows you to Unsuppress All Holes.

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IntelliShapes

Search IntelliShapes based on the size (or Based equivalent Volume), you can click on the cube with the arrows to detect the dimensions of the part selected in the scene. It allows to Suppress (Unsuppress, Select or Delete) smaller or larger IntelliShapes of the stated values. It allows you to exclude from the search Blends, Chamfers and Drafts

Color

Search for parts by color, you can click on the color preview to select the color of the selected part in the scene. It allows to suppress (Unsuppress, select or delete) equal or different parts with the indicated values (R, G, B and tolerance).

It allows you to create a Configuration from the result of the selection.

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Set Smoothness

This tool let you setting the Surface smoothness for all parts of the scene (or active selection), drag in scene and enter a value to specify surface smoothness of facets.

Difference between smoothness 10 and 50

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Double Bend

The Bouble Bend Tools is similar to Add Curved Stock in Sheet Metal catalog, the difference is that this tool add an parametric double bend, so you just have to enter the required values for add it at existing sheet metal.

For edit the values, right clic on intellishape and select Modify DoubleBend Parameters…

Double Bend example:

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Config by Property

The Config by Property tool allows you to create Configurations based on certain Custom Data present in the elements of the current scene.

The dialog box is divided into three parts, the upper one there are icons for deleting, adding or removing the custom search rules, an icon to save the search presets, and a combo box to choose presets saved; in the middle, the grid with the customdata to search inside the scene, and at the bottom a text field to specify the name to be assigned to the configuration.

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Export Elements

This tool allow to export a part or assembly to multiple formats at once.

Drag the tool onto the part (or into the scene, to export selected parts or assembly) and select the files formats.

The left side of dialog allows you to select the file formats to be exported, while the individual tabs set the options for the chosen formats.

At the bottom of the dialog box, you choose how to construct the file name and destination folder.

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Face to DXF

This tool allow to export a face of part to a DWG/DXF file.

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Operativity

• Drop the tool on to the face of the part with the left button, select the destination folder and the dwg/dxf format. (the file name is the same as the part name)

• Drop the tool on the part face with the right button to open the dialog where you can choose options:
  • Select Faces
    • you can export an additional 2D sketch shape
    • with hold the Shift key, add or subtract other faces
    • select all parallel faces to the first choice
    • select all coplanar faces to the first choice
  • Settings
    • options for the file name, if it is a SheetMetal part and how to write the data in dxf.

After saving the file the result will be shown. (If you check “Execute IPROCadViewer after export” they will be opened in the CAD viewer ).

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The settings and info to be written to the dxf file are also found in the IPROSettings dialog.

Profile to DXF

This tool allow to export a section of intellishape to a DWG/DXF file.

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Operativity

Drop the tool onto the intellishape of the part, select the destination folder and the dwg/dxf format.

(the dxf file name is set with the part name)

After saving the file will be shown the result.

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The settings and info to be written to the dxf file are also found in the IPROSettings dialog.

Create Params by Excel

This tool allows you to import parameters from an MS Excel sheet and assign them to the part in order to drive it.

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Operativity

• Drop the tool on the part to which you want to assign the parameters, choose the cells of the parameters and their values.

• For Edit params

  • Right click on the part and choose Open MSExcel file that controls the Parameters… to open the file directly.

• For Update params

  • Right click on the part and choose Update Parameters controlled by MSExcel or use the tool Update MSExcel Parameters.

• For Show params

  • Right click on the part and choose Show Parameters Controlled by MSExcel… to open the dialog where you can view the associated excel file and the cells used,

  

  by clicking on the folder or file cell, you can choose a new excel file from which to take the parameter to be associated with the field.

Create ProActive Parts

PROActiveParts is a powerful tool useful to manage parametrical parts. PROActiveParts allow you to set and incapsulate into a parametrical part all the values related to the parameters. These values are indexed by the PartNumber. Furthermore also CustomValues and a Preview Picture can be set and stored inside the parametrical part.

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When a parametrical part has been transformed to a PROActivePart, the user can change it double cliking on it (or right click and choose Add-on Properties).

How to create and manage PROActiveParts

In order to create a PROActivePart, you have to create a parametrical part. Here is a Parameter Table related to a simple parametrical part:

When it will be transformed in PROActivePart, all the parameter values owned by the Part D1, d, Dm, L and T will be managed by ICMechanical.

How to create PROActiveParts

To start the PROActivePart tool, drag the “Create PROActive Part” item from the Tools catalog, and drop it over the parametrical part. In alternative, you can select before the part, then drag and drop the item in the scene. This dialog will be displayed:

How you can see, the columns of the grid in the dialog are PartNumber, Description and the names of the parameters defined in the part (only those contained in the part are shown, and only the free ones, i.e. without expressions that bind them to others). At this point the user can fill the grid with all the values related to parameters, or he can import them from an external MSExcel file.

Before to evaluate the import/export functionalities, we will describe the commands available on the dialog box:

This group of buttons allow the user to create, rename or delete the groups grid.

This allows parameters to be managed in different grids (called Groups); which will be shown in the part selection dialog.

This group of buttons allow the user to move, insert or delete the rows of the grid.

This group of buttons are used to add, remove, rename and update a Custom column in the grid, add color, and load or add new parameters.

Custom columns are used to set values that will be transferred to the CustomData of part. User can add and delete these columns, but he cannot add or delete columns related to parameters or BOM Information.

This button adds a column to define color; it is useful for associating a color to be applied to the element related to each record.

This button shows a dialog with the names of the parameters associated with the part, you can then add them all to the grid, or just the selected ones.

How you can see, every column has an icon that describes the type of data.

This option is used to define in what Unit of Measure are to be considered the parameter values inserted.

This text box is used to assign a name at the ProActive Dialog, and will be visible at the top of the dialog.

This option is used to select the Material for the part.

The buttons included in this toolbar are used to create, select an existing image and preview the Picture to be associated to the PROActivePart.

These buttons are used to create a 2D drawing (based on a chosen icd model) for each row of the table and export them to pdf or dwg files separately.

These buttons are used to import or export the data contained in the grid. Using the import functionality you can import all the parameter and custom values from an existing MSExcel file.

As example, here is a valid MSExcel table that you can import:

How you can see, the first row contains all the Names related to the columns. During the import, every column name will be evaluated and associate to the correspondent parameter name. Every column that will not match with a parameter, will be managed as Custom Data. In the above example, the columns “Supplier” and “Note” will be Custom Data.

After the import of the above MSExcel file, the dialog will similar to this image:

The user can still edit any value, add or remove any Custom column and move change the order of the rows. If the user double click on the Row Counter, the values of the parameters in the row will be transferred to the parameters in the part.

When the user clicks on Apply or on the OK button all the information on the grid, and the Preview image will be elaborated and stored inside the part. In other words the part has become a PROActivePart.

At the bottom of the dialog box are two tabs for management:

In addition, one or more cells in an Excel file can be linked to the fields.

The user can also create complex expressions (based on the data extracted from the part) to assign to variables or use to fill in the properties.

This button is a simple help to explain the use of tags in cells:

• @ means any numeric parameter value can be entered manually, insert a value after @, it will be use as default.
• [...] means that the user can choose from a series of defined values, the values must be inserted between the characters [ ] and must be separated by a semicolon ;
• <...> means that the parameter value can be entered manually between a min and max value, the values must be inserted between the characters < > and must be separated by a semicolon ;

The last button activates automatic sizing of the grid columns. If the user clicks it, the columns fix the current size.

Operativity

When the user double click on a PROActivePart, or when he drop it inside a scene, this dialog will be displayed:

Using the PartNumber option (and/or other group options if present), the user can select the type of part to use, and all the parameters and customs will be filled with the right values.

Also, if you click the Data button, the dialog will expand and you will see the grid containing all the data and you can select and apply the values by double clicking on the grid:

In addition, if the user clicks on the Settings … button, the On Drop dialog will be opened and you can choose how to display the ActiveParts dialog box; the choices are:

• Always
• Only when you release in the background
• Never

Edit data

This button allows you to position all the elements contained in the grid by applying all the values in succession, when you click, a dialog appears to define how to position the elements in the scene.

This button activates automatic sizing of the grid columns. If the user clicks it, the columns fix the current size.

This button allow you the edit the data contained in the grid. If the user click it, the dialog described at the beginning of this page will be displayed.

It is also possible to hide some columns; this operation also hides the values in the dialog box.

Set MsExcel Parameters

It allows you to assign the value of cells of Excel files to the parameters of a part.

Operativity

• Drop the tool on the part,
• A dialog box appears with the available fields (parameters), click on the Folder or File cell and select the Excel file,
  • A new dialog box appears showing the Excel sheets,
• Select the cell you want to assign to the parameter and confirm.
• Repeat for each field you want to assign.

At the end of the operation close the dialog box, an icon with the fx symbol appears near the anchor to indicate that an excel file is associated with the part.

For Show params

Right click on the part and choose Show Parameters Controlled by MSExcel

For Update params

Right click on the part and choose Update Parameters Controlled by MSExcel or use the tool Update MSExcel Parameters.

For Edit MSExcel file

Right click on the part and choose Open MSExcel file that controls Parameters… to open the file directly.

Update MsExcel Parameters

This tool allows you to update parts that have parameters controlled by Excel file cells (assigned with Create Params by Excel and Set MsExcel Parameters)

Operativity

Drop in the scene to update.

Elements along 3D Path

With this tool you can position an element (part, assembly or intellishape) along a 3D curve or 2D sketch.

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Operativity

• Select the element and the path (curve or sketch),
• Drop the tool into the scene.

In the dialog, set the number of copies, the distance (or even distribution) and if necessary the offset.

It is also possible to change the orientation in tangency along the curve with respect to the X and Z axes of the element anchor (each click on the arrow rotates the object in steps of 90 ° with respect to the chosen axis).

The positioning of the element along the path is done with respect to its anchor, as well as rotations.

Replace Element

This tool allows you to replace one or more elements with another from an external file or present in the same scene.

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From external file

Operativity

• Select the element (part or assembly) to be replaced and then drop the tool into the scene,
• select the file you want to insert,

In the dialog box displayed you can set how to replace elements:

• all linked elements,
• or only the selected element.

Elements that have the same PartNumber:

• all the elements,
• only elements in the same parent (assembly).

Elements that have the same UserNumber:

• all the elements,
• only elements in the same parent (assembly).

The inserted element will be automatically linked to the original, if you don’t want it, you can unlink it after replacement.

Replace in place

If you want to use the tool to replace elements with an element present in the active scene, release the tool with the right mouse button,

the dialog box is similar to the previous one but allows you to choose the element to be used for the replacement directly in the active file.

Operativity

• Select the element (part or assembly) to be replaced and then drop the tool into the scene with the right mouse button,
• set the element replacement mode,
• select the element that will replace the previous ones.

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Insert Element

With this tool you can insert an element from your library of files into the scene.

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Operativity

• Drop the tool into the scene.

In the dialog box, you can, in the first combo box, select the User Library folder that contains the element you want to insert,

then in the second combo box, select the item you want to insert.

Create Tabs and Slots

This tool allows you to add tabs and slots to both sheet metal and innovative parts.

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Operativity

• Drop the tool on the edge you want to add the tabs to.

In the dialog box you can select type and set the dimensions:

in the first combo box, select the type of tab you want to add,

See here for how to add your Tab.

Placement

Here you can choose the type of placement between:

• Evenly Spaced - choise of copies and distance calculated automatically
• Distance Spaced - choise of distance copies auto
• Fixed Spaced - choise of distance and copies
• Center Spaced - choise of distance and copies from centre
• Edge Length - equal tu the edge
• Custom - choice of distance between each tab
• Custom & Length - choice of the distance between each tab and also of the length of each tab

The distance and the number of tabs vary according to the choice of placement.

Offset

In this section you can set the starting and ending offset, the icon on the right allows you to swap the start and end.

Dimensions Tab

Here you can set all the dimensions based on the chosen tab (so some boxes may be inactive).

• Length of the tab.
• Height of the tab.
• Reduction of the tab height (but not of the slot).
• Round/Chamfer size.
• Radius of the hole at the base.

Slot Type and size

In this section, you chose type and set the clearance spaces around the tabs, these are the dimensions that will create the slot hole on the opposite element.

The padlock on the right allows you to enter values that are all the same.

(The size of the cut boundary is represented with a semi-transparent yellow shape)

Edit Remove and Update Tabs

To change tab settings, select an IntelliShape-level tab, right-click IntelliShape and select Edit Tabs.

Similarly, if you want to delete all the tabs on the border, right-click IntelliShape and choose Remove Tabs.

If the element has changed size (thickness or dimension), you can update all tabs in the part, right click on the part and choose Update Tabs

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How to create a new Tab

In order to create your tabs and slots, the models must be parametric, and be saved in the folder of the library.

Here are two example of Tab and Slot:

Tab1.ics is a part with a one parametric section:

The IntelliShape named Tab creates the tabs on the element on which you drop it, and must contain these parameters:

• L - corresponds to Length of the Tab
• H - corresponds to Height of the Tab
• R - corresponds to Round or Chamfer if present
• RH - corresponds to base Hole Radius if present

Thickness isn’t present because it’s calculated from the element on which the command was dragged.

Slot3.ics is a part with a one parametric section:

The IntelliShape named SMDrill creates slots on the neighboring element on which the tab is released, and contain these parameters:

• L - corresponds to Length of the Tab
• TH - corresponds to the tolerance to be added to the height
• TL - corresponds to the tolerance to be added to the length
• RC - corresponds to base Hole Radius if present

W = Thickness it’s calculated from the element on which the command was dragged.

Update Tabs

Update all elements with Tabs&Slots.

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Operativity

• to update all elements in the scene, drop the tool into the scene.
• to update only one element, drop the tool on the element.
• to update only the elements of a selection, first select the elements, then drop the tool into the scene.

Create Explosion

With this command it is possible to create different types of exploded views, which are saved in the configurations.

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Operativity

• Drop the tool into the scene to create an exploded view of all elements.
• To create an exploded view of only the selected elements, first select the elements, then drop the tool into the scene.
• Now drag the slider or type the explosion percentage, and dynamically see the result.

Options

The icons at the top allow you to:

• Set a new selection to explode:
  • useful for redefining the elements to explode from now on.
• Remove items from selection…
• Add items to the selection…
• Show active selection:
  • useful for seeing the elements that are subject to the explosion.
• Show TriBall in the center of the explosion:
  • useful for redefining the center point from which to start the explosion.

You can explode elements from:

• the center of the footprint of all elements
• following the Z direction of each element (Z is the long green whisker on the Anchor)
• following the negative Z direction of each element

Explode Assembly to treat as Part: if you check this box, you also explode the elements in these assemblies.

Configuration Name: set a name to the configuration to assign to this explosion.

Create Explosion Lines

Tool to create, show, suppress or delete explode lines of an Exploded configuration.

The lines can be continuous or dashed.

Operativity

• Drop the tool into the scene and set the lines.

Views Manager

Useful tool for saves and restores camera status, active configuration and item visibility. This tool also stores the suppression status of the elements. It is a kind of “enhanced” Camera and Configuration Save, with a preview image and some text fields to use for documentation. All this information (images and text) can be exported to an MSExcel or MSWord document.

Operativity

1. Drop the tool into scene,
2. Adjust the view, hide or suppress unnecessary elements , or select the configuration and then click Save Current View/Configuration,
3. Add view title, description and note,
4. Repeat step 2 and 3,
5. Export to MsWord or MsExcel,
6. or save all images in one folder.

The buttons are used for:

• Move the saved view Before or After,
• Save the current view,
• Update and save the selected view,
• Delete the current view,
• Set the size of the image to be saved,
• Export the History of Views,
• Export all images in one folder.

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In the left side of dialog there are a buttons for:

• set the target camera,
• use TriBall for set target point,
• set the view orientation with Z axis,
• set angle of rotation view,
• buttons for rotation by angle,
• set step of pan view,
• buttons for move view by step.

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Import Profiles from Scanner

Import and manage points from the scanner.

Operativity

• Drop the tool into scene, and choose file to import:

• automatically generates profiles,

• and creates an extrusion or loft from a selection of profiles.

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Regenerate Scene

Similar to the Regenerate tool in Tools/Operations Ribbon, but in this case it regenerates all elements of the 3D scene without making any selection.

Operativity

• Drop the tool into scene.