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