I taught Inventor classes for years, and I have often said that I have learned much more teaching classes than I ever did taking them. That is because at some point I had answered all of my own Inventor questions, but I had not answered everyone else’s questions.
This happened to me again last week. The question was simple: What is the best way to constrain fasteners to holes in a curved sheet metal part?
The problem with a curved sheet metal part is that the holes are curved. They are no longer true cylindrical holes, but are deformed into ellipses because of the sheet metal deformation. The Inventor constraint tools do not recognize the ellipses as geometry to constrain to. The Mate constraint does not even pick up the centerline.
I struggled with this for a while. Then I realized that I had to create some reference geometry to constrain to.
First, I used a tool that is not commonly used in sheet metal design: Surface patch. This tool creates a surface using edges or loops. I created patches for the square and the circular holes in the part.
Next, I created work points at the center of the patches using the “Center Point of Loop or Edges” option of the work point tool.
Finally, I created an axis using the Normal to a Plane through a Point option. I could select the newly created surface patch and the work point as reference geometry.
Now I have a point and an axis, perfect geometry for using the Mate constraint to constrain fasteners into the hole. This technique worked well with both the round and the square holes. The video below shows the steps that I went through.
If any readers have a better technique, please share it in the comments below.