Hi, I want to apply a surface cut to a body to further reduce the volume (weight) of a part. I would like the cut to carve out a dome-like shape from the part while maintaining tangency to the existing face near the edges of the cut.
In the picture below, the boundary sketch that should define the edge of the cut is highlighted.
How can I make this surface so that the surface cuts evenly?
draw a point in a 3D sketch somewhere in the part that represents the peak of the dome. Then make a Fill surface from the sketch boundary with the point as the constraint sketch. Then use the boundary sketch to extrude a surface out of the part. Then knit the extrude and the fill. Then use Insert/cut with surface.
Matt - Nice simple technique, though when I tried it on a sample part there's no way to achieve tangency to the surface as per Alex's request. It's not possible because '...tangent constraints cannot be applied to patch boundaries containing sketches..'.
As an acknowledged expert, have you another simple technique to achieve tangency (other than simply adding a fillet to the resulting edge!)?
Cheers, Keith
Update: Couldn't load Alex's part to see the possibility of adding a fillet his part as it's a future (so must be 2011) version...
Love using this Matt, mainly 'cuz my brain doesn't wrap itself easily around a 'fill surface' tool to create the geometry described. Thanks!
Alex, et al,
I have attached a sample of how to do Matt's method, although I've simplified it quite a bit. My version does not require converting to a surface body. For those of you not running 2011:
Create a surface fill of just that sketch.
Create a sketch of the point that you want the "domed" surface to maximize at. I made a 3d sketch with just one construction line and one point, directly below the origin. You can create multiple points if you want.
Create another surface fill, this time selecting the outer edges of the flat surface body created by the fill. Set the edges to tangent, and select the sketch you just created as a constraint curve.
Hide the flat filled surface. Use replace face, and select the existing face to replace, and select "domed" surface as the replacement. Fini.
Charles - an elegant solution and really obvious once done! I should have thought more. Thanks.
Awesome, I was able to get it to work using Matt's method. I had offset my sketch from the edges of the extruded cuts, though because it was throwing an invalid geometry error when I went to do the surface cut. Might be something related to zero thickness geometry
I'll give your method a shot, Charles
Your method worked great too, Charles and I didn't have to offset the surface to avoid the geometric condition error. It wouldn't let me mirror the replace face feature across the midplane between the two large flat surfaces, though (after I adjusted the dome depth to be less than half the thickness of the part) - I had to mirror the domed surface and use replace face on the other side.
It doesn't surprise me that mirror feature didn't work. You should try mirror face instead. Use the mirror command, but select a "face" instead of a "feature". Note that after you create a feature pattern, you cannot change it to a face pattern. You must create a new pattern feature.
Proof that sometimes we actually make what we design
Alex!
Thanks for posting the pictures, I missed that!
I am working on a presentation now for "surfacing tools for nonbelievers" (I'm giving it in KC and Omaha in a couple weeks), and I'm going to include those in there. Thanks!
Charles
draw a point in a 3D sketch somewhere in the part that represents the peak of the dome. Then make a Fill surface from the sketch boundary with the point as the constraint sketch. Then use the boundary sketch to extrude a surface out of the part. Then knit the extrude and the fill. Then use Insert/cut with surface.