Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:

  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Lots of errors doing basic things with imported DXF

jesjimherjesjimher Member Posts: 2
Hi

I've imported a DXF file into a sketch and it shows fine as a (I think) a closed loop of splines:



 I can extrude it without problems, but now I need to create an offset around it, and no matter how I do it, Onshape ends up with errors. I've tried using sketch offset, and while preview shows it fine, after I confirm the operation it runs red and doesn't work saying "could not offset entities". I've tried using "offset surface" on the extruded sketch, but while most faces offset fine, some of them make Onshape show everything as red saying it's not possible:



I've also tried sweeping a circle alongside extruded object's contour, without success:



Am I missing something, or it's just that Onshape doesn't manage sketch splines that well? it's getting very frustrating, no matter how I try it it just doesn't work, and for no apparent reason (that I can see).

Here's the document link if somebody needs to look at something: https://cad.onshape.com/documents/9811b06bd9877e005a533cfb/w/ed15e9ffe4d53d9b55d56392/e/a9823598b68956503ca73fdb

Thanks!

Comments

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 1,919
    Hi @jesjimher - yes they are splines, but I am guessing that there is an issue with the tangency between them which would cause offsets and sweeps to have self-intersecting geometry. Try creating a new sketch drawing a single closed spline using the points from the first sketch.
     
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • owen_sparksowen_sparks Member, Developers Posts: 1,997 PRO
    That looks pretty symmetrical so you could possibly model 1/4 of it and them mirror the result twice.
    Production Engineer
    HWM-Water Ltd
  • Cris_BowersCris_Bowers Member Posts: 99 PRO
    edited February 6
    This is the same situation I have run into with most of the DXFs I have to import into Onshape. A workflow I have found helpful is after importing your sketch is to fix everything in place, all the points should show up as blue but the lines should be black. Then accept the sketch. Now create a new sketch on the same plane and select the "use" feature and select inside the imported sketch region. All the problem areas will show up as red, while the rest will be black. Now open another instance of the part studio in a new window. You can now join all the points of the failed geometry and it should fix your problems. It's tedious, but until they come up with a way to auto-join points from imported DXFs it's the only way I know to use.

  • dick_van_der_vaartdick_van_der_vaart Member Posts: 45 PRO
    I have the same problem with importing DXF files with logo's.
    When working with Adobe Illustrator or Coreldraw for converting the logo from a vectorfile, AI. or EPS the export is not usable, lots of small segment's.
    The solution I've found is simple, use Inkscape, that's open source software similar to Illustrator.
    There are some tweaking checkboxes for exporting or save as DXF but the result are perfect.
  • Cris_BowersCris_Bowers Member Posts: 99 PRO
    @dick_van_der_vaart I will have to try Inkscape. Our art department uses Coreldraw. I export those files to .eps then clean that up in another program before exporting to DXF, which I then clean up further in AutoCAD. Obviously I am still doing some more clean up in Onshape.
  • jesjimherjesjimher Member Posts: 2
    Thanks everybody, I finally solved it by following @NeilCooke advice. I deleted everything from the DXF but the points, and drew a new spline over them. Had to manually create a sketch point for every DXF point, but at least it works.

    By the way, the DXF file came from Inkscape (it was the result of vectoring a bitmap). Perhaps I messed up with vectorization settings, though DXF looked fine.

    Thanks again to everybody, I didn't know what else to do, and you gave pretty solid advice.
  • michał_1michał_1 Member, Developers Posts: 202 ✭✭✭
    This is a problem that might be unsolvable, and I mean "vector graphic" software > cad, workflow as a whole.
    Import/export fails on import mostly because cad software "can't read" knots until broken. If cad brakes them on import then it's fine,  when don't user must do that before import.
    Another way around, from cad to vector software, most common issues are caused by NURBS curves or primitives like circles and ellipses. Both can be turned in to beziers.
    These problems can be addressed either by developers or users specific practice.

    The biggest issue is that even when we succeed with data translation imported curves can be unusable, especially when we try to offset either outline or extruded body.
    Reason for that is what is known as "near tangent". Smooth/symmetric knots are equivalent of tangent constraint between sketch entities but the way they are written in vector software is not enough precise. When recomputed in cad they are no longer tangent, what's worst, just slightly but enough for computation to fail.

    Few tips you can find here:
    https://forum.onshape.com/discussion/comment/49555/#Comment_49555
Sign In or Register to comment.