Trying to design a Pyramid in sheet metal environment, as I sketched my last side (Tab) the following failure message appeared: Face printing operation failed!
I have redrawn my sketch to create the tab and the message keeps popping up, telling me to edit my inputs. What is going on? What should I do? Any help would be greatly appreciated.
Solved! Go to Solution.
The part is failing because of material interference on the right side of Tab 7.
Here is a picture of where your tab profile sketch ends: (At the very corner)
Here is a picture of the flange corner from an angle. You can see that the tab you intend to create intrudes upon the material of the opposing end of the base wraparound band. Also, you can see that I pulled the Tab 7 profile away from the corner and the software created and bent it fine.
The zero thickness/non manifold issues with trying to create material all the way into that corner are what is causing it to fail, even if it doesn't state this specifically. In fact, if you only pull that Tab 7 profile corner back a few thousandths, it actually changes the error message to zero thickness/non manifold.
A simplified explanation of this behavior is that creation of tabs, flanges, etc cannot violate material boundaries, while flattening and bending operations can. This is how you created an intersecting corner that only failed when you went to add a tab in that area.
I attached a similar example file of how to make this a bit cleaner and more manageable to edit. This would keep your bend radii, important pyramid flap dimensions, etc, in a single feature, so that a change to the desired geometry doesn't force you to make the same edit across multiple features and increase the chances of an error.