I am trying to cut out a business logo using the Advanced Vcarve toolpath in Carbide Create Pro (Build 764).
I have the toolpath configured to use a 1/32 em for the pocketing operation and a 60 degree v-bit for the carve. When I run the job, the em only cuts the pockets in the top of the letters but never attempts to cut the key contours.
Should I be using the full depth of the material for an Advanced vcarve operation like has been suggested for a vcarve operation with a 60 degree v-bit?
What is the proper configuration for an advanced vcarve for this type of file?
Advanced V-Carve is meant to have a flat bottom and is usually used when the features being cut are wider than the Vee-bit. Advanced usually doesn’t need to be very deep (0.025 - 0.050), unless you want a little more shadow / contrast on the edges of the letters.
You are carving deep enough that there aren’t very many flat areas, and they aren’t big enough for the clearing bit. If change the depth to something like .05", then that remaining areas are large enough for the clearing bit and it gets used.
The clearing bit is only used for flat areas left when the VBit traces the perimeter of the design - the clearing bit doesn’t go around the vectors of the design.
Looking at your file, the only reason I can see for the end mill not attempting to cut the key contour is that the key contour is in a separate toolpath group than the advanced v carve and both the key contour group and toolpath are disabled. The key contour toolpath and group both have to be enabled for the contour to be cut.
It seems like you have some redundant toolpaths with two advanced v carves ( one shows as a 45 degree and the other a 60 degree v bit). If you go with the 60 degree bit (and it is at least as wide as your widest letter -about 0.33 inch), due to the width of your letters, the depth will max out at ~0.3 inch with either V carve tool path. Entering any depth greater than this will have no impact on the depth of the v carve. If that depth is acceptable, there is no reason to limit it nor is there a reason to go with advanced V carve unless you just want a different look. If that is too deep, limit it with an advanced V carve with or without a pocket clearing tool. Never limit a plain V-carve toolpath-it will look bad. With a plain v carve toolpath you are better off reducing the width of your letters or switching to a bit with a greater angle, both will effectively reduce the depth but still yield an acceptable carve.
For your design, I would go with a 60 degree bit, plain v carve toolpath for the letters. The key contour toolpath is independent of the v carve.