I am trying to pattern a solid swept cut around the face of a cylinder, the preview while still in the Circular Pattern feature shows the pattern I want but whenever I hit the green check-mark to actually build the feature I get an error saying that the pattern failed.
I need to use the solid swept cut for this feature as it is important that the walls of the cut remain normal to the surface throughout.
It should work. Can you post the part file?
Here it is, the goal is to have the pattern appear 8 times around the circumference and then I plan to finish the rest of the part.
I'm seeing the same thing you described. Maybe because it's intersecting itself when patterned? I rarely use swept cuts, so maybe someone who's more familiar with them can help. I'm sorry I couldn't.
Inspired by Glenn's theory of self-intersection, I tried cutting a hole through the center of the part and then patterning, hoping that would eliminate self-intersection. But it still didn't work. However, if you eliminate self-intersection in such a way then you can pattern faces instead of features, and I was able to get this to work. I don't know what the end result is supposed to look like, but if you were going to have a bore through the part anyway then maybe patterning faces after the hole might work. See the attached model.
In my understanding and practice......The patterns are still parametric in that if you try to pattern a swept cut, you have to be able to sweep the cut with the existing geometry. You will see this a lot when trying to pattern fillets. All of the intersecting geometries as Glenn indicated, make it impossible. For something like this, you would be best creating your features you want to cut as un-merged solid bodies. Then pattern the solid bodies, then perform a combine, subtracting the solid bodies from the main solid.
Craig,
Cheating....in a sense, but it allows you to change your cuts all day long, keeping your end result totally parametric...
Only took a minute to do.
Let me know if this is the desired result.
Yes that's exactly what I was trying for! Thanks for helping me out!
In my understanding and practice......The patterns are still parametric in that if you try to pattern a swept cut, you have to be able to sweep the cut with the existing geometry. You will see this a lot when trying to pattern fillets. All of the intersecting geometries as Glenn indicated, make it impossible. For something like this, you would be best creating your features you want to cut as un-merged solid bodies. Then pattern the solid bodies, then perform a combine, subtracting the solid bodies from the main solid.