How to bend a whole assembly out of different materials?

SOLIDWORKS How To Questions
1

For sandwich assemblies we would like to bend the whole assembly to get the correct flat pattern for all the parts. Is that somehow possible?

The assembly itself is made out of a frame of tubes, some galvanized sheet metal pieces in between, styrofoam in between the frame & wooden pieces that cover the whole frame. Is a multibody part the only viable option here? Or is there another way?
The frame out of tubing was originally designed as a weldment, but we are willing to take a new route here too.
Maybe a skeleton part, that defines the bending is the solution?

Edit for clarity:

Here the swamp link.

I colored them to distinguish them better:

  • Inside (i.e. wood) Layer 1 blue
  • steel plates Layer 2 green
  • frame/ styrofoam/ other insides Layer 3 frame: grey, styro: red
  • steel plates Layer 4 green
  • Outside (i.e. FRP) Layer 5 yellow

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2

It’s possible with a multi-body part, or a skeleton part but I’d most likely go with a multi-body part for this.

Depends on what you’re working with and how much context you want with it too. If you want the part to work across multiple sub-assemblies then skeleton sketch part might be more suitable.

3

Master Sketch with correct ID OD rad for each piece.
Unless you can have gap at the bend.

4

The drawing will be made out of

  • a weldment frame
  • styrofoam to fill the gaps
  • galvanized steel parts at various positions on top/at the back of the styro/weldment
  • a finishing layer for both sides (wood/metal)

production needs the measurements on the flat pattern of each piece, but for assembling it later on we need the finished position after bending this sandwich.
For the weldment, the driving dimension is the finished total height. According to this they need to cut/drill/torch the pieces in the flattened state.

I’ll try to give you a simplified example soon.

5

OR use the right tools for the right job! NX Laminate Composites. Sorry guys..SolidWorks is still a mid-range software..people need to realize there is a limit to what you should do with this tool vs what it can do. Then determine if the can-do process is worth the effort and maintenance.

6

bump, because I heavily edited the first post

7

Not sure if I got it..

You could do an assembly, then create a new part inside the assembly with Join feature, thus making a kind of multibody. Then use the Flex feature to bend (?)

Is not possible to make the bended parts with sheet metal? I think would be easier.

8

I’ll try and respond when I get some free time. Maybe mattpeneguy can give you a quick summary of how to do it with a skeleton part.

9

so we tried it out with the following:

weldments for the frame & the flat steel parts combined with a skeleton part, that defines the bending. We used the flex feature for those parts. I am sure we did several things wrong, but this is our first tryout with a skeleton part.

This worked, although the auto-trim didn’t work as well as expected for the frame. it looks great too & it’s faster than our old purely mated assemblies.
Regarding the drawings: weldments are kind of an odd thing, especially if you have bent pieces in there. After the Flex feature, you have ‘new bodies’ in the weldment part, which creates a BOM nightmare currently. part A has a different BOM number in the bent configuration, so any change order weould be fairly confusing now (‘Change part A’ - and now you have to know which version they are talking about, because part A (flat pattern) is part C (bent).).

THE GOOD

  • weldment cut lists are amazing for the purely cut parts & save a ton of work
  • just changing a sketch to adjust positions or just add something to a weldment is amazingly easy
  • we actually have the parts at the correct position in the bent configuration, currently this is not really accurate in our drawings, because we only have a flat pattern for i.e. the steel parts in layer 2/4
  • it’s faster, because there are just a few mates

THE BAD

  • our BOM guys hate the mess, that bent weldment parts create
  • Adding a weldment body to a drawing is very tedious & does not seem to be very error prone (change of body results in a lost drawing - all measurements are gone too!)
  • structural member automatic trimming did not work very well & it’s hard to see which parts need trimming (possible place for mistakes)
  • for outsourcing & due to company policy we would need to use save body to send out some tubes to get lasered (I really don’t like save bodies, but correct me if I’m wrong!)
10

What does he hate? It certainly is a different way of working, and might cause drawings to be heavier, but there’s nothing extraordinary that differentiates it entirely from the rest

How do you process? When creating a drawing view, you can select the desired body to display, we’ve never had issues with this before, so I’m not sure how this would cause issue for you. Do you have an example? I’m guessing your parts require more dimensions then just the overall dimensions.
Here’s an example of ours:
image.png
What I did/do hate is that you need a different cartridge for multibody parts because you can’t have body property callouts inside drawing templates, so we have a cartridge for multibody and add all the cartridge information by drag and dropping annotations on the view so that they link themselves to the body.

Not sure I’m understanding this, I didn’t have too much trouble with the whole trimming thing, but I certainly haven’t used it to the extent that you have.

That, I can understand, I don’t like saving bodies either. Perhaps configs to display the body and save each configs as body names?

11

What does he hate? It certainly is a different way of working, and might cause drawings to be heavier, but there’s nothing extraordinary that differentiates it entirely from the rest

They work with the order of the items in the BOM. Changing the order creates them a lot of work. It may be just this case, but the order of the items changed regularly when we made changes to the parts (because they are ‘new bodies’).

How do you process? When creating a drawing view, you can select the desired body to display, we’ve never had issues with this before, so I’m not sure how this would cause issue for you. Do you have an example? I’m guessing your parts require more dimensions then just the overall dimensions.
Here’s an example of ours:

Exactly. You select the body to display. If the body changed (i.e. through adding a feature) it got lost. Plus, selecting the body from the view screen looks nice, but why can’t I just select every single body from a table?

Not sure I’m understanding this, I didn’t have too much trouble with the whole trimming thing, but I certainly haven’t used it to the extent that you have.

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we had to manually trim those, because it did not recognize the interference there. Since we use SW 2017 SP5 ( >>> ) we can not yet use detecting interferences on a part level.

That, I can understand, I don’t like saving bodies either. Perhaps configs to display the body and save each configs as body names?

I thought about that too, but then again, we would loose the benefits of the weldment again. We don’t want to have 10 different configurations of one part (makes it huge & slow). But I will keep it in mind.

If we can fix the BOM problems, we will switch to the new style for sure. It’s so much faster & easier to modify, that we can live with some hiccups.

12

I think bending the parts in assembly is not a healthy method.
After I draw each part one by one and assemble the assembly, I make the necessary arrangements in the assembly (angles, holes, welds, etc.). flex is not a healthy command for me, at least for sheet metal, controllability is important to me because every part is produced. (the illustrations are not just for visual purposes.)
I deal with details in assembly, sometimes I use auxiliary lines. Just being visual is not enough for me, it should be manufacturable.
my examples are sound insulation, styrofoam, various coatings.
I do not know the details of your work, but this is my opinion that you can act in a controlled manner.
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