I’m trying to figure out how I can have an angled cut path with a 60 degree vee bit going from 1/8" deep at one end of a X axis to 1/4" deep in a straight line along the same X axis about 4" from the beginning. Is this possible? I know it takes some time to draw it up using a different software package than in Carbide Create.
This is not possible in Carbide Create.
You can sort of do it by drawing segments, each of which cuts to a different depth, then having a final toolpath which one edits in the G-code to cut at an angle if the steps aren’t acceptable.
I actually use this as an example in a project I’ve been working on:
but it’s not to a usable state (in particular, it needs to have a robust way to handle multiple passes), and I doubt anyone else would be interested in it, and it’s currently getting re-written (again), this time in pure Python (which can then be called from OpenSCAD if desired).
The real work-around for this would be to model the cut in 3D using Carbide Create Pro or some other 3D tool.
Seems pretty possible to me…
Draw a 0.072" radius circle. 4" away draw a 0.144" radius circle.
Connect the tangent points & unite, or trim & join.
Run a V-carve with a depth per pass deeper than the total depth.
8 Likes
@Tod1d, That is brilliant!
Easy on that “brilliant” stuff!! 
To be fair, it’s not a very pretty toolpath, and it has a few corner picks (sewing machine moves).
Way cleaner to create a contour no offset on a 4" line at 0.125 deep, then just add the one Z value at 0.250.
(Design File: )
(stockMin:0.000in, 0.000in, -1.000in)
(stockMax:6.000in, 2.000in, 0.000in)
(STOCK/BLOCK,6.000, 2.000, 1.000,0.000, 0.000, 1.000)
G90
G20
(Move to safe Z to avoid workholding)
G53G0Z-0.197
(Toolpath: Contour Toolpath 1)
M05
(TOOL/MILL,0.125, 0.000, 0.000, 0.00)
()
M6T102
M03S10000
M0
G0X1.0000Y1.0000
Z0.0098
G1Z-0.1250F8.0
X5.0000 Z-0.250 F20.0 (Add the Z here)
Z0.1575
M05
M02
Steve,I have to agree with you that is Brilliant from Tod.Trying it now
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.