Hi,
I want to create a 3d sketch to trim certain part of the object I have. So I created points on the 3d surface and then connected the points using 3d spline on surface. However when i use this sketch to use as a trim entity, it gives me an error (see image attached). I am not sure why it says that the 3d sketch doesnot intersect. Any insights on this or work arounds for this situation? How can I check if my 3d sketch is coincident on the surface or not?
Part available here.
Thanks
Frank Krockenberger. Yes, I understand that is a way to work around this. But why is the 3d spline on surface not working like it should. What am I missing?
Thanks
You'll see if you create the extrude, but only extend it up towards the Front plane, that it won't cut because it doesn't intersect with the original surface body. This leads me to believe that you have gaps between the spline and the surface.
I think it must be a bug. SW will let you create an intersection split line with that spline, and as far as I know the same rules apply for creating an intersection split line with a 3D sketch (sketch must lie on the surface).
You already know about the workaround by creating an extruded surface, but in case you are interested another workaround is to create a split line with your spline and then delete faces to remove the faces on the upper side of the split line.
Looks like the spline ends are coincident to the surface edges? I've had trouble with similar situations and ensuring the surface is extended out past all sketch edges/points usually will solve the problem. Just a thought. ;o)
Hi.
You can try to start a new sketch on front plane. Then project your 3d sketch with Convert Entities to current sketch and use this as trim tool later.
Nisha,
Using your 3d spline create a extruded surface and use that surface as your cut surface.
since it is a 3d spline you will have to specify the direction of the extrude.
Frank