I’m hoping someone can help. I’ve created an STL file for an object designed to be 18mm thick, and I’ve imported it into Carbide Create Pro to cut on Shapeoko 3 CNC at a 1:1 scale.
The issue is, when I simulate the toolpaths, the cut depth shows it going way under the expected 18mm thickness — it’s not cutting deep enough, and the shape looks compressed vertically.
I’ve double-checked that the material is set to 18mm thick, and the STL itself is definitely modeled at that height. But something seems to go wrong during import or toolpath generation.
To help explain, I’ve attached:
The STL file
A screenshot of the actual product I want to make
A simulation screenshot showing the issue
Any help or guidance would be greatly appreciated!
Is the top portion the correct height? It looks like maybe it’s just not cutting to the bottom. Offset the outside boundary by the radius of the tool & use that as your boundary for 3D toolpaths. The boundary has an “ON” condition, to the center of the tool will stop on the boundary. To machine to the bottom of a near vertical surface the tool needs to be allowed to machine outside the part. In fact, to get all the way to the bottom it will also need to be allowed to machine the tool radius deeper as well.
“ON” condition means the tool stops with the tool center ON the boundary. A “Tangent” condition would stop the tool edge on the boundary. So if the boundary is on the edge of the part, the tool can’t cut low enough to finish the outside near vertical wall.
In Carbide Create Pro you would also need to increase the Stock Thickness and the part height by the radius of the ball-nose tool if using a ball-nose for cutting out the perimeter — but probably MeshCAM would be better suited for this part.
