Flat pattern for virtual parts

SOLIDWORKS
1

I have an assembly containing several virtual parts. I create a display state (“01”) where all components are hidden except for a single virtual part.

I add a drawing, insert standard views (Front, Top, Right) and assign display state “01” to those views. This allows me to generate a drawing for that specific virtual part directly from the assembly, without saving them as external parts.

Is it possible to also show the flat pattern of this virtual sheet metal part within the same drawing too?

Thanks.

2

There is an open SPR requesting this ability:

SPR618141 - Ability to create a drawing with flat patterns for all the bodies of the part or all parts of the assembly in one drawing

The only workaround I can think of is to create a configuration in the part (called ‘FLAT’ for example) with the flat pattern unsuppressed and then create a configuration in the assembly (called ‘ALL FLATS’ for example). In this assembly configuration, set the configuration of all the parts to FLAT. Then you can create a view in the drawing using the ‘ALL FLATS’ configuration.

It’s not a great workaround. The bend line sketch has to be shown manually, and then it disappears sometimes and a rebuild is required to see it again. There are no bend line notes. But if you just want a flat pattern that you can dimension, it works.

4 Likes
3

Thanks.

Will give it a try. Seems promissing.

4

Ok I gotta ask. If the part needs a flat drawing view (I assume to be manufactured), why would it be virtual? Wouldn’t it be a seperate part with its own drawing?

3 Likes
5

That worked.
Million thanks.

6

The answer to this question is quite complicated, and it absolutely goes back to our rare situation, but I’ll try my best to explain a part of them.

First, we don’t design anything. Our customers provide us with drawings, and we manufacture parts based on those drawings. So we always start from the supplied documentation.

Most of these drawings are for sheet metal products made up of 100+ parts, welded or spot-welded together. You can think of each final product as an assembly consisting of tens or hundreds of sheet metal components.

To manufacture them, we first need to create the individual parts. Using SolidWorks, we build 3D models based on the received drawings, then export DXF files and send them to CAM software for production.

About 99% of these parts are never reused in other assemblies. So, if we receive an order with drawing number “AAA” that consists of 10 components, instead of saving each part separately (AAA-01, AAA-02, etc.), we create a single 3D model named “AAA” that contains 10 virtual parts. What’s the benefit of having 10 files with slightly different names, rather than one assembly with 10 virtual parts?

In very very rare cases, however, we decide to create separate drawings for specific parts to make things easier on the shop floor. for example, when a part is particularly complex or requires additional details for bending, inspection, or other processes. (But it’s really rare)

On top of this, when an assembly consists of around 50 components, SolidWorks (at least in our experience) performs better when using 50 virtual parts rather than opening 50 separate files.

I’m aware of options like Lightweight or Large Design Review, but virtual parts still seem to work more efficiently for us. In any case, we rarely need to create separate drawings for these parts, except in very rare situations.

3 Likes
7

We use a mix of techniques and I think that the virtual components approach is the least bad. performance wise. I do no think there is a 100% good approach.

We also have some very big multibody welded “part” with up to 1400 bodies and the performances are atrocious. making a drawing is almost impossible, but we have some smaller multibody part that is quite fast and the approach is not that bad.

the real issue is when you want to import some existing 3d data from outside the multibody part. Inserting a part into a part is full of bugs, let alone if you use the copy move body command.

Using an assy solves that issue, and it is more logic than stuffing a lot of unrelated bodies and semifinished weldments together in the same part. Assy approach has a big advantage in terms of performance since its components are not fully opened all the time, since the assy shows only the parasolid data without the overhead of the underlying parameteres.

Using virtual parts, they need to be read from inside the assy ("unpacked”) and written into the temp folder in a real file, then read again in SW. Plus the backup copy at every save operation if you have that option turned on.

If you have lot of virtual components it could cause quite some overhead with disk operations. And we had some (rare) case in which temporary files from a virtual component got deleted (probably during a crash or a OS related hiccup) and the assy was left corrupted without some component.

I decided to disable the backup and autorestore since it seems lighter, and less demanding making SW more stable imho.

Since cutlists can be used with assemblies, I am trying to implement a mixed approach with the assy, a main body as virtual component and external files inserted and oriented to form some sub weldments.

But it depends a lot on the data you need to make. And the way of thinking of your engineers.

3 Likes
8

Fortunately we don’t have assemblies as big as your 1400+ ones, but when the number goes up, we have a macro to stop auto rebuild of the assembly. Once a virtual part is finished and we are working on another one, there’s no need to rebuild the whole assembly. Once an edit is necessary, a manual rebuild does the job.

1 Like
9

I suppose you can mix the two and just externally save the sheet metal parts you need DXF drawings for and leave the rest virtual. If you don’t want to jump through the assembly, configuration hoops to get them on the drawing.

2 Likes
10

I recall a time when making a sheet metal part that the flat pattern was made in the part at that time. A few years ago I was getting back into sheet metal parts and the flat pattern configuration was not added till it got put into the drawing. Sounds like you get to have lots of fun working on others parts.

1 Like
11

Depends. Here we have sheet metal starter templates for common shapes (flat plate, L, U, etc.). You can have the flat already created however we ended removing it due to always having to rename them to the part number.

It’s been long neglected omission that SolidWorks still hasn’t added a right click option to add the flat configuration using their naming convention.

1 Like
12

@mp3-250 Do you also have drawings for your virtual parts? If yes, would you please explain how you make your drawings? Do you use display state like I explained above, or do you use other methods?

Thanks.

You can always use a macro. A click on a button will do the job.

13

For some of our jobs, the virtual part is used inside an assembly and the assembly has its own drawing with a cutlist that includes the body in the virtual part. So the drawing looks like more as a multibody part than an assembly.

We do not have the necessity of flat patterns. our suppliers do them for us the right way, since most of our sheetmetal models are approximations.

As a general rule we try to avoid display states, because we found them hard to control and sometimes unreliable. We use mainly configurations for our assemblies and no configuration is allowed for parts.

SW2025 introduced a new (configuration like) interface to manage the show-hide setting at the component level so it could be more convenient to switch to display states instead of configurations in the near future, but for the time being I would stick with configurations.

1 Like
14

Thanks.

1 Like
15

This is still correct, but if you open a drawing & drag the flat pattern from the view palette onto the drawing sheet & then close the drawing without saving anything, the flat pattern configuration will be created in the part file.

1 Like
16

I’ve been doing Sheetmetal more than 15 years and never have experienced that.
Either I’ve been lucky or Solidworks likes me.

Do you happen to start from solid and then convert to sheet metal?

17

I just about always start with sheet metal features, but I do not think that it matters. I do not have a flat pattern configuration until I create a flat pattern in a drawing. I’d try to create a video of what I am talking about but I’m not very good with videos.

1 Like
18

I just tested this and can verify that it works as @DLZ_SWX_User describes. Here are the steps I performed:

  1. Create a new part using a plain vanilla empty part template
  2. Create a simple sketch and create a sheet metal base flange feature
  3. Save the part
  4. Create a new drawing
  5. Select the part model in the view palette drop down
  6. Drag the flat pattern from the view palette on to the drawing
  7. Close the drawing
  8. Examine the part and you will see that the flat pattern config has been added
3 Likes