Glenn Schroeder

Using Plate in Weldments

Discussion created by Glenn Schroeder on Jan 28, 2015
Latest reply on Jan 10, 2019 by Glenn Schroeder

I've referred to using Plate in weldments on several Forum posts, and a member contacted me about sharing my files, so I created this Discussion in case someone else is interested.

 

For some background, a few years ago I created a folder with some plate profiles (simple rectangle sketches, centered on the origin, with additional points for alternate insertion locations).

This allows me to use the Structural Member function on the weldments toolbar to create Plate instead of doing it with Extruded Boss/Base.  By doing this the cut list properties (description, length, angle, etc.) for Plate are generated automatically by the software just like they are for Square Tubing, Channel, W-sections, etc., which saves a great deal of time.

 

I only created a few of the probably infinite number of plate sizes, but when needing Plate I just pick one that's close, then close out the Structural Member function, expand it, and edit the sketch to the needed size.  Since weldment sketches are copied when used for Structural Members and not linked you can edit the sketches in the Part without affecting the .sldlfp files.

 

 

The Description property is linked to the dimensions, so it will update if the sketch is edited.

 

 

[2019-06-19 Edit:  I was just reviewing this and remembered something.  If you have a circumstance where you want other factors to drive the width (or thickness) of the plate, after creating it you can edit the profile sketch inside the Part, make the desired dimension Driven, then fully define the sketch with relations.  By doing that the size will update to match edits farther up in the tree, and the Description property will update accordingly.]

 

You can use the attached file for plate, editing the dimensions after inserting the feature as described above, or use it as a template for creating more sizes (just open it, change to the desired dimensions, and "Save as..." to a new file name).  If you'd rather use configurations I've attached the Plate file.  It only has three configurations now, but more can easily be added.  I didn't bother with an Excel-based design table.  Instead I saved a simplified table.

 

You can open the table and add new configurations as needed.  The configuration specific Description property will automatically be generated, with the correct dimensions, for each new configuration.

 

I was also asked about my criteria for multi-body Parts versus Assemblies when using weldments.  If it gets welded together, then I create it as a single part.  This includes nuts or other hardware that's welded to structural steel, which is one of the few times I ever insert a Part into a Part.  I know some people will break a multi-body part into separate parts and re-assemble them into an assembly when finished.  That's certainly one option, but I never have.  The "Select Bodies" button in Drawings makes it very simple to detail separate bodies.

 

Any bodies that get bolted together I create as separate parts in an assembly, but there's really no reason they couldn't be modeled as multi-body Parts also.

 

By the way, I've also created a folder with round profiles.  It works very well for rebar, cable, etc.

 

[2018-08-31 Edit:  I've recently revised my workflow for Plate, and am updating this accordingly.  I deleted all the files in my "Plate" folder, which had more or less random thicknesses and widths, and replaced them with a single file for each thickness (they're all 2 inches wide).  Of course, after creating the feature I almost always need to change the width, but I was pretty much always doing that anyway.  This way the name of the feature in the tree isn't showing the wrong size after the edit, and I have fewer files saved in the .sldlfp Plate folder.]

 

 

  I deleted the file I had previously posted here, and replaced it with the "0.2500" file.

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