Flat Pattern DXF Export Issue

[pavmed]

Hi!

I've stuck with this. I try to make outline to cut oracal sticker which in turn goes onto profiled sheet metal.

My workflow:

1. Make target sheet metal profile in Sheet metal workspace. I use custom Rule with .1 mm thickness.

2. Get sticker outline sketch with such an angle to metal sheet that I want it to be read correctly. In this case 45 degrees.

3. Extrude -- Cut this sketch through metal sheet

4. Then I make flat pattern (goes ok) and when I try to export DXF I've got this 'unexpected problem'

One else guy reports the same issue with this workflow. Other sheet metal models do not generate this error. 

I've examined metal sheet edge after extrude and found this artefacts:

So obviously this workflow has a flaw but I cannot understand how to overcome it.

Any ideas? 

Now we have workaround without DXF export involved.

My model with download permission -  http://a360.co/2CLdpZ2

[paul.clauss · Accepted solution]

Hi @pavmed

Thanks for posting! I think the inability to create the DXF is due to the off angle cut through the part as well. I have a couple of workarounds that may help.

The first workaround would be to take your part, as is, and project a sketch of the body (in its flat pattern state) to a new sketch on the top face of the flat pattern. You could then save the sketch as a DXF, but it will not include the bend lines. If you need the bend lines in the DXF, you would need to create two DXF files - one from the flat pattern before the cut (for bend lines), and the other from the projected sketch. 

The other option would be to create surface bodies from the perimeter of the letters, use them to split the faces of the folded model, and then extrude the splits after creating the flat pattern. This will allow you to use the Flat Pattern DXF export as intended, as it will ensure the cuts run straight through (are perpendicular to the top face of) the flat pattern. Big kudos to Jeff S. and Phil E. for their help with this method!

I've shown both of these options in the screencast below - please let me know if you have any questions.

[pavmed]

Hi Paul!

Thank you for your answer. 

I see the issue is that angle cut body lines cannot be exported to DXF automatically.

I've also tried with 5 mm metal thickness - it helps to get rid of artefacts but still couldnt help with DXF export, it gives the same error.

And yes, currently I use the first workaround you described. 

The second one illustrates that straight cuts export works OK.

The only thing I would add to first workaround is that sketch one use to project cutted body should NOT be placed on bodys face to avoid double lines (known project issue).

Instead it should be places on any plane - origin or offset. Or you can place skecth on body face DO NOT project anything on it, then close sketch and save it as DXF and it will contain all that base face line in it.