Adding geometry to cut as a pocket with a finishing pass

(William Adams) #1

One technique which is often suggested to avoid slotting is to add geometry around a part which one wishes to cut out and cut as a pocket down to tab depth — here’s one technique for that.

In this case, the project is a bevel gauge which will be cut out of 0.0625" (~1.5mm) thick aluminum:


Due to the narrowness of the angles, an 0.03125" endmill has to be used, so after importing and scaling the file (we will be cutting out one which is 3") we select the perimeter and offset it twice, once by the desired chipload (0.01") and again by half again the endmill diameter:

(control click on the profile, then delete the extraneous bits of path left in the centers of the divots)

Setting up roughing and finishing pass in CC
What CNC bit used to cut out letters
Uneven Depth of Cut issue
Uneven Depth of Cut issue
ShapeokoXXL: Backlash and bad circles issues
How to generate toolpath?
3/4” Bowl Bit Issue
CarbideCreate/Nomad cut size slightly wrong
Cutting Name Necklaces with Nomad on Brass (0.8mm thick)
3XXL 6061 Machining
First aluminum fail, figuring out why
Small groove where endmill plunges
First Cut - Weird Issue
What Drill bits to use?
So here's a new one to me
(William Adams) #2

Select the offset paths and assign a pocket operation:

Note the Depth Per Pass and set the depth of the pocket to leave the desired tab thickness, in this case, twice the 0.098mm depth per pass.

(William Adams) #3

Select the original path and assign a cut from stock top down to stock bottom, adding tabs as desired:

(William Adams) #4

Add toolpaths for the text and holes, then preview to verify, then make G-Code and cut.

(William Adams) #5

Cutting in aluminum w/ a #122 we’ll need feeds and speeds. There is an example of this at:

These settings are:

  • Depth per Pass: 0.102mm
  • Stepover: 0.356mm
  • Spindle speed: 9200RPM
  • Feedrate: 190.068mm
  • Plungerate: 25.4mm

(William Adams) #6

Managed to get it cut, but had to use Grbl’s feedrate override to finish the cut:

(Allen R Curry) #7

Some Questions…

You said a technique to avoid “slotting.” What is slotting?

You added two offsets. Why two and what was the rational for the offset distances?



(William Adams) #8

Slotting is cutting a slot just as wide as the endmill will cut — a follow path / Contour | No offset cut into the material — the tool is engaged along the entire leading edge of the cut (a half-circle).

The two offsets allowed one to cut a pocket which would leave a “roughing clearance” adjacent to the material. Then one can make a finishing pass to take off that last thickness of material to get to the final dimension.

(William Adams) #9

Available at: