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How can I make an embossment that ist cut by the edge of the part?
I have to transfer a sheet metal part from SolidWorks to Onshape.
The part has several embosses, some of them cut by the edge of the part.
In SolidWorks there is no real problem - it adds material beyond the edge when you add the embossment, you cut it off afterwards - problem solved.
SolidWorks:
Working with Onshape, no matter what I try, nothing works…
If I try to add the embossment like in the first picture, the embossments that cut the edge aren´t added at all, you get errors shown etc.
If I add material, so that the embosses don´t cut the edge, I can add them, no problem.
But if I cut this material off afterwards, the embosses are removed and are shown as errors, doesn´t work either.
Onshape:
I´m used to having to use workarounds to make things work in Onshape, but this time I don´t know what to try in addition to get a part that looks like it should and leads to a correct flat pattern.
I suppose you can make special embosses only for this part or something like that, but that can´t be a serious solution, wasting too much time.
Can anyone help?
Answers
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I believe this is a hard limitation with the tool registration functions in the engine that disallow form features to extend past the sheet boundaries of a given sheet metal surface body. I've experimented with trying to modify the form tool to work on non-planar faces and across bends but all of these attempts were unsuccessful. @lana would know best though.
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That is indeed a current limitation of sheet metal Form feature . You can remove the extra material after Finish sheet metal - then it is all baked into 3d, but it will remain in flat pattern.
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Yes, making the 3D model work is not a real problem, that works comparably good as in SolidWorks.
But we also need a DXF to manufacture the part.
As we obviously have to deal with this flaw indefinitely we tried to find a workaround for the DXF.
It´s too time-consuming and hand-knitted for my liking, but it works.
Beginnig at the very start, first you have to add enough material to make the embossment work at all:Then you can do the forming of the sheet metal:
After that you can finish the sheet metal part (that´s a sheet metal feature) and cut off the surplus material like you would do in any other part studio:
Btw: Just look for the red points in the following images!
Now you generate a DXF from the flat pattern of this sheet metal part.
Of course this flat pattern isn´t correct, that´s what we´re talking about here:Choose what should be included in this DXF:
Now yout get the DXF with the unwanted bulges:
Create a new part studio:
Start a new sketch.
Click the "DXF" icon and choose insert DXF or DWG:Choose the DXF with the unwanted bulges:
This way you got a new sketch derived from the DXF:
Now you can edit the unwanted bulges:
Do a right click on the sketch and choose export as DXF / DWG:
Now you got a DXF that looks like your part in real life - beside the fact that the hole in the embossment is still missing, only the bend lines are shown:
If you want to make a drawing of the flat pattern, you have to generate an additional part studio, import this edited DXF (see above) and make a solid part of it.
Of course all lines that depict bend lines etc. have to be converted into discontinuous lines before.
And if these bend lines should be shown in the drawing, you have to display the sketch in addition to the part.
Of course you have to add the bend lettering (up or down, radius, bending angle) manually now.
Best way in my opinion to add the right values is to generate a depiciton from the original flat pattern and put it beside the drawing sheet as a template for the hand-knitted edited version.
This way you can also check if there were changes to the part when you open the drawing in the future.
Because I don´t think this drawing will update automatically…0


















