A question that regularly pops-up is about how to create cut-outs in Inventor for a part that is sticking through a sheet metal part.
When the penetrating part is perpendicular to the sheet metal face it penetrates, there is no issue as you can use the regular "Cut" command.
But what if the penetration happens under an angle like in below image of a cylindrical part?
The cutout will have to be wider than the cylinder diameter to avoid interference.
It is relatively easy to determine mathematically what the width W of the opening needs to be.
I'll spare you the gory details on how exactly I got to these formulas but here they are:
Width of opening = d1 = Thickness / tan(TOOLANGLE) + TOOLWIDTH / sin(TOOLANGLE)
Height of opening = d7 = TOOLWIDTH (the Height of the opening is rather arbitrary and can even be made smaller if required).
TOOLANGLE = the smallest angle between the penetrating tool and the sheet metal face. This angle is always <= 90 deg and > 0 deg.
TOOLWIDTH = maximum cross-sectional dimension of the tool when it penetrates the opening
With this knowledge, I decided to create three iFeatures. The three different cutout shapes are circle, oblong and rectangle.
You can download the metric 2012 part that I used to create the iFeatures here (so you can build more shapes if you like)
You can download the finished 2012 iFeatures here and use the "Insert iFeature" command rather than the "Cut" command for situations where the regular sheet metal "Cut" command is not giving the results you want.
Here is a snapshot of the 3 cutout shapes in action. Note that the cross-section of the penetrating parts can be an irregular shape different from circle,oblong or rectangle.