Export Sheet Metal to DXF only saves sketches for single body parts?

[mike miller]

I have gone around and around with this one; suppressing sketches, editing flat patterns, editing map files, etc. ad nauseum.

It seems that SWX will export sketches just fine as long as there is only one body in the part. As soon as there are >1 bodies, it will still export geometry and bend lines but not sketches. If I create a Delete/Keep Bodies feature, and leave only one, it works fine. Any ideas?

@Roasted By John
@Glenn Schroeder
@mattpeneguy

Trailing Arm.SLDPRT

(375.16 KiB) Downloaded 45 times

[bnemec]

I have gone around and around with this one; suppressing sketches, editing flat patterns, editing map files, etc. ad nauseum.

It seems that SWX will export sketches just fine as long as there is only one body in the part. As soon as there are >1 bodies, it will still export geometry and bend lines but not sketches. If I create a Delete/Keep Bodies feature, and leave only one, it works fine. Any ideas?

@Roasted By John
@Glenn Schroeder
@mattpeneguy






Trailing Arm.SLDPRT

I cannot open your file (2019) but I've been working with dxfs for laser lately so did some testing on multi body. Here's what I've found: Always with the "Sheet Metal" radio button selected

-Only unabsorbed sketches show up in dxf
- If there is more than one body only the first shows up (geometry checked), doesn't matter if there is more than one body in the selection box.

image.png

Sorry for the dumb question, but why would you want multiple bodies in one dxf and also sketches? I'm assuming this is not the one part number per file use case? Or piece parts do not get part numbers?

[mike miller]

I do not want more than one body in a DXF. I want one body along with any sketches that are shown in the Flat-Pattern configuration.

[jcapriotti]

Does the same thing in 2021. Not that it helps but.......SolidWorks shows it fixed in 2022, SPR #931297

As a workaround, you could suppress the features so you only have one body, then it works. With a bit of rework you could isolate each part's features in folders for easier suppression, but that doesn't work well when one part needs to reference another, which is the reason I assume you are using a multi-body sheet metal part here. You can get around that by having a single skeleton sketch to reference instead of the parts to each other......again...a bit of rework just to get around a limitation on dxf export. But not bad modeling practice either so.....

[mike miller]

Does the same thing in 2021. Not that it helps but.......SolidWorks shows it fixed in 2022, SPR #931297

As a workaround, you could suppress the features so you only have one body, then it works. With a bit of rework you could isolate each part's features in folders for easier suppression, but that doesn't work well when one part needs to reference another, which is the reason I assume you are using a multi-body sheet metal part here. You can get around that by having a single skeleton sketch to reference instead of the parts to each other......again...a bit of rework just to get around a limitation on dxf export. But not bad modeling practice either so.....

Noice. I have no plans to downgrade any further, so no thanks. (not aimed at you, @jcapriotti )

The only workaround I've found is Delete Bodies. Suppressing doesn't help...

[jcapriotti]

Delete bodies is good and better than the rework I mentioned.

[KevinC]

Not in front of SW at the moment to test, but what happens if flatten and then save as>DXF using an annotation view?
Do the sketches get included?

Kevin

[mike miller]

Not in front of SW at the moment to test, but what happens if flatten and then save as>DXF using an annotation view?
Do the sketches get included?

Kevin

Yeah they do. But it won't work for us. Even selecting Flat-Pattern View has the same result.

image.png

[KevinC]

[quote="mike miller" post_id=1279 time=1616417923 user_id=118]
[quote=KevinC post_id=1250 time=1616358582 user_id=111]
Not in front of SW at the moment to test, but what happens if flatten and then save as>DXF using an annotation view?
Do the sketches get included?

Kevin
[/quote]

Yeah they do. But it won't work for us. Even selecting Flat-Pattern View has the same result.

image.png
[/quote]
What about creating an unfolded config?

[bnemec]

Not in front of SW at the moment to test, but what happens if flatten and then save as>DXF using an annotation view?
Do the sketches get included?

Kevin

Yeah they do. But it won't work for us. Even selecting Flat-Pattern View has the same result.

image.png

I could be way off here, but I don't see how the SaveAsDXF could do this as it's likely there are sketches on other, non-parallel, planes. I think the DXF operation can only be given one set of x,y,z rotations and offsets, so I'm thinking it cannot include the sketch from bodyA that may be on the front plane and put it on the same 2D dxf as the sketch for bodyB that may be on the side plane. If we orientate the DXF to bodyA (front plane) and get the sketch, then the sketch for bodyB would just be a line, or a stack of colinear lines, if displayed on a 2D dxf aligned to the front plane.