I have an imported part from a customer. I added sheet metal to it and everything looks good until I flatten it. The radius doesn't flatten out right and I am not sure why it is doing this. Any help is appreciated.
I have an imported part from a customer. I added sheet metal to it and everything looks good until I flatten it. The radius doesn't flatten out right and I am not sure why it is doing this. Any help is appreciated.
Peter,
This is indeed curious. It took me a bit to even see the conflict you are talking about. For the benefit of others reading this thread here is the scenario:
1. Imported part and zoom on one corner
2. Same smooth bend after inserting bends
3. Notice shape after Flatten-Bends and before Process-Bends using the rollback bar. This shows the flat pattern as it should be.
4. Compare to the flat pattern generated. Notice how the edge is straight through the bend. The straight edge goes from corner to corner of the bend tangency.
This is very weird.
This can be fixed by editing the flat pattern feature and turning off 'simplify bends'.
Thank Josh
Josh Helman wrote:
This can be fixed by editing the flat pattern feature and turning off 'simplify bends'.
THANKS! I did not even know that was there!
Edit the Flat-Pattern3 feature in the DefaultSM-FLAT-PATTERN configuration and uncheck simplify bends to get the spline along the bend to show in the flat pattern configuration.
So the unchecking simplify bends works but why should I need to do that? Is there a scenario that I would want it to simplify bends so the flat isn't what it should be? I found that in the document properties under sheet metal you can uncheck simplify bends there for a part template, but is this going to cause other problems in the future?
It simplifies the flat pattern which some companies like and seems to be easier on lasers and such when you transfer this data to your lasers software.
I came to know that curved edges can increase the manufacturing cost that is the reason simplified bend option is there to get straight edges.
Peter Muesch wrote:
So the unchecking simplify bends works but why should I need to do that? Is there a scenario that I would want it to simplify bends so the flat isn't what it should be? I found that in the document properties under sheet metal you can uncheck simplify bends there for a part template, but is this going to cause other problems in the future?
The processing of the flat pattern is dependent on how it's being manufactured. Certain profiles are easier on different processes; is the part being stamped out, water cut, lasered, routered? What processes are going to be done to the part after the bends; welded or is it if finished at that point. The true answer is the ambiguous one that no one else can answer for you: Design Intent.
This part is laser, form, and weld. The design intent is to fit over another part but since Solidworks added material to the radius it no longer fits and I have 200 rejected parts.
If I cut away material on a part, why would I ever want Solidworks to add material back in the flat? On this part it added .230" at middle point!
This pic is 2 parts over each other. One with simplify and the other not.
It would be nice if the formed part looked like the flat pattern when using simplify bends. 
This can be fixed by editing the flat pattern feature and turning off 'simplify bends'.