On one part, I have a bore hole drilled on a curved surface so the hole is actually an ellipse.
Now the other part I am trying to constrain together is the pipe that will be welded into the bore hole; so that is a simple circlular pipe.
The issue is that the pipe has to be inserted 0.25" above the interior of the bore hole to allow for room for the weld. In order to do this I have tried to create a plane attached to the 3D ellipse and then constrain the pipe to be 0.25" above that plane. The problem is I cannot seem to create a plane attached to the 3D geometry; I cant even find a way to attach points, or pick the center point of the bore hole.
This is a really frustrating aspect of the Inventor Software.
Can someone help me figure out how to create a plane on 3D geometry and link it to said geometry.
I'm using 2012, if that is necessary information.
Vijai Christopher Sookrah
Mechanical Engineer, EIT
Aircraft Appliances & Equipment Ltd.
Solved! Go to Solution.
Open the file with the hole.
Create an axis in the hole.
Create a workpoint at the implied intersection of the surface and the axis.
Create a workplane at the intersection of the workpoint and axis.
Now you can use that as an offset constraint in the assembly.
Attach your assembly here if you can't figure it out.
The work features created in the part are not showing up in the assembly.
Does the fact that the part is an ipart and the assembly an iassembly make a difference?
Hi! For iPart, if you want to have the work features in iPart factory to show up in iPart members, you will need to explicitly add the work features to the author table with "Include" flag. After that, the iAssembly containing the iPart member will need to be updated and then the iPart members will have the work features.
Please try it and let me know if it works.
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