Hi People
I'm kinda new in SolidWorks.
I have an assignment where i need to make a revolve cut. But i can not make it work.
It given an error "operation failed due to geometric condition.
I need to remove the top and the bottom part, so that i only have the blades in the middle.
Hope someone is able to help.
I think part of the problem might be that the sketch you drew for the axis is not actually the center of rotation of the part so it's creating thin sections when it tries to cut. You could create an axis using the ID bore instead. But then the axis doesn't lie on the plane that you sketched on so you might need to use a different plane to create your sketch.
All that said, I tried sketching on the Top plane instead, using Intersection Curve to get the geometry to cut, and it still doesn't work. I guess there is something weird about where the blades meet the rest of the part.
Do you need the result to contain the entire blades? If you just need it pretty close I'd suggest offsetting your sketch by a tiny bit to cut away some extra material and that should take care of any infinitely thin sections that would result. However I don't think you can offset a fit spline so you might have to create your sketch using converted entities rather than a fit spline. Then you could offset the entire profile.
After squaring up the cut face with the bore (as Jamil pointed out), and recreating the profile sketch, here's what I get with a revolve cut, probably not what you're looking for.
Looks like you changed something in your sketch after the cut revolve after it worked once, probably since you got a result close to this?
Instead of doing a revolved cut, try doing a revolved surface first and then do a Cut With Surface. Also, use Convert Entities rather than a Fit Spline to make sure your sketch follows the edges correctly.
Extend your sketch lines past the part, and just have a single open profile. Add your centerline axis into the sketch, and it should revolve just fine. Once it is revolved, Cut With Surface and keep the main body only. Repeat for the other side of the impeller.
On the other side, I actually had to use a Thickened Cut as I'm guessing there was some zero thickness geometry causing an error. A bidirectional cut with a thickness of .01mm worked for me.
Patrick this is ecxactly what i need.
This surface thing how does this work ?
The surfacing tools work very similar to the solid modeling tools, you are just creating faces only with no thickness. Right click on the Command Manager tab and turn on the Surfaces toolbar to gain access to them.
One thing to remember is that when using surfaces to make cuts, always make sure the surface extends past whatever it is going to be trimming.
Could it really be that surface cut, isn't existing in the student license version of solid works.
I really can't find that feature??
Sorry for the stupid question
The student license is fully functional.
You have to right click on the tabs and load the Surface toolbar.
In the upper right corner of your SolidWorks window is a search bar. Use the dropdown to select Commands, and then search for "Cut with surface".
Maybe I'm just stupid.
But i cant make it to work.
This is what i have right now, and i can't make the cut
There is a problem with the converted sketch entities in Sketch4. I'm not really sure why you offset a plane and then converted entities, as that just creates the surface in the wrong location. Also, the endpoints of the sketch entities do not intersect. If you zoom in really close, you can see there is a gap between the endpoints. This is causing the revolve to create three surfaces, rather than one.
Start a 2D sketch on the "cut" face of the part, then use convert entites on the edges of the part. When you are connecting the arcs, pay close attention and make sure they all intersect completely. After you create the revolve, look at your Surface Bodies folder and make sure only one surface was created.
So I tried to get the Revolve cut to work. Is this what your trying to do?