A colleague and I are working on a large assembly together, and we have received several .stp files from a customer (originally created in ProE), many of which are sheet metal that need to be unfolded and flat patterns made in drawings. The sheet metal default thickness has been changed to what the material thickness is. We have measured the edges on each side of and the radii of the bends, and they all appear to be consistently uniform. Yet, we get an error when trying to unfold or flatten the outer two bends. The customer sent us a flat pattern .stp file as well after letting them know we could not unfold the part, and there are many dimensions that we have to manually inserted to the drawing with the flat file because it does not have the bend information in it.
Is there something that we are missing to make this part unfold all the way?
In case my signature does not attach, I am running 2011 SP2, Windows7 Pro (SP1) 64-bit, 12GB RAM, Intel Xeon 3.07GHz, NVIDIA Quadro 2000
Solved! Go to Solution.
I have narrowed the problem down to the two outer bends - but haven't found easy solution yet.
The solution can be achieved, which is to recreate the sheet metal body using Thicken command. And the flat pattern can be done.
As the dataset is large, please see the detailed steps below -
1. Select the faces to create offset surface with distance=0mm
2. Delete the base2 solid body using Delete Face command
3. Thicken the offset surface using thickness=4.5mm
4. Create flat pattern via pre-selecting one inner face
Brilliant! Thank you!
What is the difference in preselecting a surface before trying to create a flat pattern? Does it simply give Inventor a reference to unfold by?
Thank you again.
Maybe there are very few failure case on flat pattern without inner face pre-selected. So the inner face pre-selected to create flat pattern is recommended. For this case, the flat pattern can be created with or without face pre-selected in R2011.
Hope it helpful for you.