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How to save only outline of model to DXF?

Question asked by Peter Brinkhuis on May 29, 2018
Latest reply on May 30, 2018 by Rob Edwards

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Hi again

I've been working on an addin that reads in hundreds of STEP models and runs tens of motion studies per model to determine in which positions these oddly shaped parts would lie on a table. The tool spits out re-oriented models and DXF files.

Right now the DXF files look similar to this section. It includes radii and all other edges. I only need the outline of the part, because that's what a camera would see.

Does anybody know how I can only export the outline of this model to DXF? I've been searching but haven't found anything useful yet. Changing the display state to Shaded didn't help.

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Francisco Martínez May 29, 2018 2:39 PM
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I am looking for something similar,

What I have been doing is removing entities upon dxf creation inside solidworks.

When I have lots of files like you do I have to make extra configs of the parts that are de-featured so only the outlines come thru on the dxf export.
maybe my methods can help
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- Peter Brinkhuis @ Francisco Martínez on May 29, 2018 4:00 PM
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  Thanks Francisco. Both methods don't work for me unfortunately. I've tried the Defeature method, but since my model is imported there are no features to remove.
  
  I'm currently creating 50 unique DXF files per part, so anything that needs manual work is a no-go I'll go looking for some external tool in the meantime.
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Harold Black May 30, 2018 9:04 AM
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If the part is modeled from one of the standard planes, you could write a macro that creates a sketch on the initial plane and convert entities of the face and save those out as a DXF. I'm not sure what your models look like so it would be hard to make a general approach unless there are more examples to be seen.
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- Peter Brinkhuis @ Harold Black on May 30, 2018 9:45 AM
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  I can't post screenshots of the models unfortunately since they belong to my customer's customer. But they are medical bone plates, so they are oddly shaped to mimic human bone shapes. That means 3D shapes, lots of fillets, the whole shebang. I don't have the original SolidWorks models.
  
  I tried converting the faces one by one, but then you get many edges that are not part of the visible contour. I still haven't found the proper way to do it manually, so I can't even start automating this.
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  - Harold Black @ Peter Brinkhuis on May 30, 2018 10:08 AM
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    Do you know what orientation your bone plates are in for the outline? You could use the mold feature and create a parting line which you can convert to a sketch entity. The parting line creates a line(s) on the part as if you are dunking that part into paint and removing it and seeing the visible line. It uses a plane normal to the direction you are "dipping" the part.
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    - Francisco Martínez @ Harold Black on May 30, 2018 10:22 AM
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      This is a good idea, I bet the parting line with a macro would automate most of his parts.
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    - Peter Brinkhuis @ Harold Black on May 30, 2018 11:49 AM
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      Tried that, thanks. Somehow SolidWorks only recognizes one parting line in a hole. It ignores the other 20 holes and the outer contour. I can get it to finish the outer contour, but then it has troubles with the holes that are under different angles. I think the model is too complex to automatically create a parting line. I think you would need a ten-piece mold for this part.
      
      I really appreciate all the help by the way
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      - Swme Eng @ Peter Brinkhuis on May 30, 2018 12:16 PM
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        Peter, what about creating a surface plane larger than the original part at the cross section that you need and using the intersect or trim surface command to trim it to the 2d profile of the part?
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        Peter Brinkhuis @ Swme Eng on May 30, 2018 12:36 PM
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        I used the intersect function a few weeks ago for another project, but for this task I can't use the cross section. I'm really looking for the contour.
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        Swme Eng @ Peter Brinkhuis on May 30, 2018 1:27 PM
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        Peter, isn't the outer contour just the cross section from a plane on top of the model?
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Kevin Chandler May 30, 2018 12:39 PM
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Hello,

You can try shelling the part with an 0.001" wall selecting all radii and faces, leaving only the outer perimeter.
Select a view that's normal to the outline for the DXF.

I hope this helps.

Cheers,

Kevin
EDIT: Yes, it's a dual line DXF.
And perhaps predicated on having some flat along the p[erimeter.
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Jim Sculley May 30, 2018 12:55 PM
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Vote for the following SPR:
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Rob Edwards May 30, 2018 12:57 PM
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Ok Peter

Here's a process that a macro could automate...

You're not going to like it but I've done a manual proof of concept.

I started with just a faceted cube, a random 3d sketch point that creates an axis and a plane.
Think of this as your viewing plane

OK next step iterate through all faces and convert entities in a sketch
(see note later)

next

for each sketch extrude up to the plane in the direction of the plane with merge result.

You will likely get some errors.
ZTG or a perpendicular direction.

but when its done you get a nice clean silhouette

* Hopefully if you iterate through the faces and then extrude directly, you will remove many of them thus simplifying the task.

Anyway Not my best idea... but it might just work

2016 attached
Attachments
- silly-oh-et.SLDPRT.zip183.4 KB
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- Harold Black @ Rob Edwards on May 30, 2018 1:12 PM
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  Interesting approach but I just tested it on a completely smooth model, all tangent faces, and I can't convert the entities.
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  - Rob Edwards @ Harold Black on May 30, 2018 1:46 PM
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    Hi Harold
    
    good point.
    
    Not to be defeqated I used a split line with silhouette option and then converted directly to the viewing plane
    then merge extrude all sketches
    This still gave a problem for some faces but in that case I selected the outer loop and converted that..
    
    so possible but not probable
    
    2016 attached
    Attachments
    splitline.SLDPRT.zip190.4 KB
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Deepak Gupta May 30, 2018 1:38 PM
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Have you looked into this example Find Outside Edges of Face Example (VBA)
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Rob Edwards May 30, 2018 1:53 PM
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Maybe this is a doh! moment. Just reimport the dxf as a sketch and extrude all the regions to merge
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- Rob Edwards @ Rob Edwards on May 30, 2018 3:16 PM
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  Hi again Peter
  
  So I popped my simple sample in an assembly and mated it just to the origin so it was free to spin
  
  I then made a drawing and added a Top View
  I made a block from the the model edges saved it out
  then created a new part inserted the block and voila!
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Rob Edwards May 30, 2018 3:39 PM
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This is easiest way yet
especially via API
Attachments
- Recording #50.mp42.7 MB
- Sample.SLDPRT.zip76.0 KB
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