Hi, I am trying to extrude a cut offset from multiple curves. I have a 3D sketch with the shape i want but i get a error every time i try to make the cut. The screen shot will explain it more.
Ultimately this is what i am trying to create.
Have you tried or could you try making the line in the 3D sketch that you reference in the cut-extrude feature for it's direction a construction line. Then choose a plane for the cut direction if one of the stock planes is parallel to the direction that you would like to cut. If no, then create a plane accomplishing this. Off-setting the cut from that surface may not result in what you want from one feature. A portion of your sketch would be cut into the part body incorrectly nearest to the OD of the part. You may be able to accomplish this by a cut-revolve, then a few fillets and a full round fillet at the peak or crest of the cut on top of the part.
We can solve this scenario by Hybrid Modelling Concept. Kindly refer the attached file.
Do you actually want the cut to go straight down, or ideally would it be normal to the dome? The way I would do a cut like that is to use your flat 2D sketch of the shape to create split lines on the surfaces to be cut, then copy the surfaces using Offset Surface with offset=0, and then make a Thickened Cut using the copied surface.
I would create an offset surface inside the solid body. Depending on what result you wanted, you could create that surface body by offsetting it by a distance, offsetting by zero distance and moving the surface down into the body, or a combination of both. Then just do a simple extrude cut from a 2D sketch, using "up to surface" for the Direction 1 mode.
You can try using a surface body in the "From" mode, but that usually doesn't succeed.
That's a good method too. If the OP actually does want the cut to be a fixed amount in the Y direction then they could copy the surface with 0 offset and then move bodies to move the copy down in y, then extrude cut up to that new surface.
Retrieving data ...