I've got a part that shows bend lines correctly in Solidworks, but when exported to DXF show extra bend lines. Does anyone know how to fix this? Any help would be appreciated. I'm running 2016 sp 4.0.
Do you ever get this message during save-as?
maybe something from the other config. is bleeding thru.(not suppressed, only hidden)
I'm not an AutoCAD user but is the double vertical line due to the line font being used in AutoCAD? Can you upload your part and dxf?
Not sure, I think the problem is somehow related to the drawing.
This is what I get after saving your drawing files as DXF but if I make a new drawing, it doesn't happen. So probably some setting in your drawing.
Can you install DraftSight (a free tool for edit/view DWG/DXF files) and see if you still get same issue?
Tried DraftSight - still has double lines. It's not a font issue, as these are actual line segments.
I believe it's related to the drawing. If I export the flat pattern from the part, there are no double lines. Additionally, when I create a new drawing with the part the issue goes away. I might have to just bite the bullet and redo the drawing.
I have two different part/drawings with this issue. FWIW we do this type of work all the time, so I don't think it's user error.
Thanks for the help, Deepak and Solid Air.
Can you tell tell us how you are saving your dxf file? Is it made from inside the part file, or inside the drawing sheet file saved as 1 to 1? Can you add your part your exporting from?
When I use to program our cnc laser and turrets, this is the method I used:
1: Hit the flatten button or unsuppress the flat pattern item in the tree.
2: Hit save as dxf; name part as desired.
3: The tree will change command prompt. Select one of the three options below and hit the check.
-Sheet metal option will make it to the flat pattern without clicking on a face or view port. It also give you the added ability to add sketches, bend lines, forming tools, etc into the dxf file if that is needed.
-Faces/loops/edges (I recommend this one) option works by simply selecting the face of the part you want to make a dxf. So you you only want to make a dxf of a certain face without the folds added in, this is your function. It works in the boundary of vertex to vertex or edge to edge in the flat view.
-Annotation views option will make the flat pattern via the view port you currently have. Be careful on this one, if your view port angle is off, your flat pattern angle will be adjusted according.
4: Next dialog will verify what the exported dxf will look like. Here you have the option of deleting lines or holes if you need to do small editing. Once you are satisfied, hit save.
Works okay when exporting from the part. We use lots of configurations, so I make a 'container drawing', with a sheet for each configuration.
I just ran your part using my regular process though the last version of AutoCAD I have installed is 2012. I opened the DXF file using SolidWorks and was shown this. I wonder if AutoCAD is showing something else for whatever reason.
I don't Flatten the part, I just select a surface and:
Right click pop-up Export to DXF/DWG
Save As 'name'
Options R12 for maximum compatibility (although this part may be due to the fact that our programming system is 5 years old
Export Sheet Metal, Geometry, Bend lines (all checked)
I stopped flattening the parts at this point when I frequently forgot to unflatten them.
I think I boiled it down enough - found a work around. What is happening is this. When I create the drawing pages for the flat patterns, I would create the first page, then copy/paste to create the additional pages, after which I would change the configurations as appropriate. For whatever reason, SW would leave the old bend lines after the config change. The fix is to not copy/paste, but to create each individual view from scratch (so no config change is required).
Thanks everyone for the help.
That is the same way I create drawings from Configs.
If the Bendlines are dangling, try to check this setting.
I know an post has been marked correct but it did not appear to fix the issue. So here is my possible solution (possible because it worked for me, now I need someone else to test it).
1-Open the model.
2-Highlight features Edge-Flange1 to Chamfer1.
3-Right click and select Delete.
4-In the Confirm Delete dialog, check Delete absorbed features and Delete child features then click Yes to All.
5-Rebuild the model using Ctrl+q.
6-Click the Undo button.
7-Open the drawing.
8-Export the flat pattern view.
Open drawing, save drawing as dxf then open dxf.
Hi good day, I presented this same trouble and read everything in here but I noticed their is non of above. the double line appeared between the bend line is due to a flatten pattern characteristic not selected: this is the merge faces. Dear Sir Daniel, check on this option. if it is not selected (which is almost always by default selected, and I get into trouble with it) their appear non-merged faces on the bends, those are the double lines between the bend line ones have on the DXF exported file.
with merge faces selected [x]
with merge face not selected [ ]
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