What's a good way to deal with plate in weldments?

SOLIDWORKS SolidWorks FAQ
1

I attached a sample Part in which I created plate using the Structural Member function instead of doing it with an Extruded Boss/Base. By doing this the cut list properties 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. There’s an example of a .sldlfp sketch below.

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I have a different .sldlfp file for each common thickness, along with a few that I created for a specific project. It wouldn’t be practical to have a file for every possible width, so I made all mine 2" wide. After creating the plate using the weldment feature I edit the sketch that’s absorbed in the feature to match the width I want. The sketches from the .sldlfp file are copied to the Part when used for Structural Members, but the Part file doesn’t maintain a link back to the .sldlfp file, so you can edit the sketches in the Part without affecting the .sldlfp file.

The Description property is linked to the dimensions, so it will update to match the edit.

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If you want the thickness or width driven by other features in the model you can edit the sketch, make the width dimension driven, and then use relations to fully define the sketch. (Deleting the dimension instead of making it driven would mess up the property.)

I also attached one of my .sldlfp files. You can modify it to suit if you like, or use it as a template to create other thicknesses. As I said above, I just edit the sketch in the Part to get the desired width, but if you have a common size you use often I’d recommend making a .sldlfp file specifically for it so you won’t need to edit the sketch in the Part every time.

You could of course create a single file with configurations if you prefer that workflow, or if you have widths you use often you could have a separate .sldlfp file for each thickness, with a configurations for each width.

This technique also works well for other non-traditional shapes, like lumber, rebar, wire, etc.
0.7500.SLDLFP (47.3 KB)

2

Just to add on here, I’ve created some configured profiles that are managed in a DT to make it easy to add or subtract profiles.

3

Glenn Schroeder you gave me great idea for furniture design ( Wardrobes, beds, closets…) - a lot of “plates”
I am doing this in my free time , and i managed to do this with weldments. Just click where the line is , instead of multiple sketches and boss extrudes :smiley:

So much easier!

4

I mostly do plates with sheet metal. Only extra step needed is to created bounding box for the part. Then I put this into the description,

“SW-Thickness” x “SW-Width” x “SW-Length”

5

I re-use my plates a lot so I have made separate .sldprt and drawing files of them. Then I create another part which is the weldment that only includes tubes/pipes/RHS/whatever cut-stuff that doesn’t require a drawing. Now I can use these plates and weldment in .sldasm file and create a drawing that orders all the plates and cut-items (BOM type must be “intended”). My company uses ERP and this seems to be only cost-effective way to use weldments and plates (plates that have drawings) together.

6

Are these parts in an assembly or in a weldment? In either case why don’t you just add the custom properties you want to the template? For a weldment if you add it to the weldment feature the properties are propagated to all all the extrusions except sheet metal. If these are Parts then you would have them in the part template.

Maybe I’m not understanding what you’re doing.

7

Do you mean a Part template? If I was doing single-body Parts that would probably work, but I often have plate in multi-body Parts, along with square or rectangular tubing, or W-section or S-section bodies. Using this method the cut list properties are automatically generated for plate bodies like they are for the structural shape bodies.

8

MultiBodied Part or Weldment? If you use weldment all the properties put in the weldment feature are propagated to all new extrusions. See below.

So we have a “Weldment Part” Template that has the weldment feature in it with the necessary properties. When we start a part that is a weldment we use that part template rather than a regular one. Everything we extrude has those properties added to it.
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Edit to add: you can also create custom property dialogue boxes that are specifically linked to cut list items. So when you select a cut list item and it pulls down custom properties to fill in. If you’re not highlighted on a cut list item the custom property tab defaults to the custom property for the part. See below. The only reason I have “Size” as an option in the custom properties is we have options in there for “See template” or “See model”. if you enter it in the custom tab it will over write the one in the properties.

Cut list item
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Part
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Also Edit to add 2: this only works on SW 2018 SP5 or later. I only know this because I beat my head against the wall trying to make it work for almost a year only to be told “I think we need to fix that”, which they finally did in SP5.

9

I edited the original post here to insert a sample Part and to add back screenshots that got lost a few months ago when the platform had the hiccups.

10

I still don’t understand why you aren’t using the weldment property approach. All the custom properties are propagated and you can auto link dimensions from the bounding boxes. You can could even automatically link to the bounding box dimensions as long as you always created the extrusion in the correct order, first dim thickness, second width, third length and so on.

11

If that works better for you, by all means go for it, but :

  1. I was already using this method before bounding boxes were a thing. Since I already have my profile sketches set up to create plate using the Structural Member function would there be any advantage to using bounding boxes?
  2. I don’t want to have to worry about whether I created the extrusion in the correct order.
  3. Also, did you look at the Part I attached? I like having one sketch that drives the whole Part, like I did there, and that sketch was used for two totally different weldment bodies without needing to make a new one, which would be necessary if I was creating the plate with a Extruded Boss.
12

I can’t open your files, future version.

If you’re already set up then there’s not much to gain by switching. From your OP I got the impression that you were trying to figure out how to do this.

Also really depends on how you use weldments. Most of our parts end up with template drawings and the only thing we show sizes on in the BOM are things cut from bar, blocks etc. We just pull the bounding boxes for that.

By combining the Weldment Propagation custom properties for properties that will apply to all parts and a custom property tab for cutlist items for “Variable custom properties” Everything but the name is either auto filled or drop down filled in.

OTOH If you are doing a lot of “Similar plates” or have “Stock items” I think profile templates is a great way to go. We don’t do alot of that and I typically create my weldments with “Cross section” sketches that contain multiple cut list items in a single sketch.