Maslow Home Maslow Community Garden

Cutting Improvements: Ramp Down in Corners and Full Height Finish Passes


I have continued to tinker with these settings. I have elected to only use the Ramp Down feature on inside corners, it seems to work well at around a 1 inch minimum diameter.

I also still like the finishing path.

I have since discovered a setting for outside corners on the Passes tab. I have been setting the Outer Corner Mode to “Keep Sharp corner with Loop.” With this setting, the cuts will go past the outside corner and make a cloverleaf like turn before changing direction. This results in some really sharp corners without sacrificing much cutting speed.


Thanks for your work and time here. I’m finding this thread helpful, I’m interested in a finishing cut as well but didn’t know Fusion360 could even produce gcode.

@krkeegan do you think the finishing cut is worth the work? Or would you say sanding, which we have to do anyways will produce the same results?


I’m curious; how many segments are in that roundover?
if I wanted an indiscernible curve with no visible stepping, how short should each segment be?

Fusion360 uses smooth curves (NURBS) that are not segmented. It uses precision tolerance to generate the math equations that describe the curves. The MaslowCNC post processor that generates the Gcode in Fusion 360 use G2/G3 code for arcs which also does not segment the curve. This leaves it down to the firmware which I believe computes a segment size based on feed rate and command refresh interval. Which is very fine.

You can also set ‘Disable Arc’ to ‘True’ in the post processor and Fusion 360 will auto-magically interpolate the curve as G1 movements, and work everything out, generating a ton of gcode. Looking at one of my previous projects I see there were ~20 position changes for a 1/4" 90 degree arc!

When the Maslow is cutting well the arcs are completely smooth. If you really want an indiscernible curve with no visible stepping then I suggest you use a NURBS based CAD/CAM like Fusion360.


Here is my latest cut generated from Fusion360 with optimized feedrates (using defaults). These had option ‘Disable Arcs’ set to ‘True’ in the Post processor (because of G2 error in 1.2.4 firmware). The Maslow slowed down greatly when doing square corner cuts, to about 1/8 speed, which for the first time are almost perfectly square. 1/4" arcs were about 1/4 speed. The large radius circle, center, was about 1/2 speed. Transition between speeds did not jerk the sled.

Very close up on the end of the handle showing transition between straight cuts and clock/counterclock arcs. These are all 1/4" radius (for scale). The only unevenness I see is on the straight cuts which I have probably set cut to fast/deep (1/4" bit at 1/4" depth at maslow max at 32ipm). This will only need a light sanding.


I can’t believe I’m only just NOW seeing this thread. Incredibly useful info for F360 users.

The downside of forums like this is so much great info like this gets buried under loads of less-helpful conversations and posts. Wish there was a (Moderator Recommended) tab that would help to sort through it all a bit (@bar?).

Thanks again for the tips everyone.


Copy that!
Unread is not working…


I ran some more cuts today and got the best result so far. Thought I would share my settings:

Make sure to set the tool settings first as other section operation setting are base of these:

Default 1/4 Spiral upcut 2 flute from Maslow

  • Spindle speed: 10000 rpm
  • Cutting feedrate:30 ipm
  • Lead feedrate: 15ipm
  • Ramp feedrate: 13ipm

Multiple Depths

  • Max depth: 0.2
  • Use even step downs: Checked
    I often use ‘Tabs’ and set them at 0.15" height when cutting 3/4" stock. When used with 0.2" depth this works out to 4 pass cuts with 3 @ 0.2" = 0.6" and final cut at 0.15", raising up and down for the tabs, to make up 0.75".
    ‘Use even step downs’ optimizes the cut depth and often reduces it when 0.2 is not needed which results in smoother cuts.

Feed rate optimization

  • In each operation settings e.g. contour, pocket
  • Uncheck ‘Only Inner Corners’ - Important: Greatly improves accuracy on all curves by slowing down cuts.
  • Reduced Feedrate: Use defaults, This seems to self adjust based on the curves in the piece being cut.


  • In each operation settings e.g. contour, pocket
  • Turn on and set tolerance to 0.002".
    Greatly reduces gcode on interpolated cuts such as lead in/outs, Bore, and complex curves. I saw reduction from 47K to 22K lines. I searched for Maslow accuracy/tolerance and could not find a definitive setting. I set it to 0.002" because I though I saw it somewhere in firmware/ground control. This can probably reduced as I doubt Maslow can achieve this tolerance.


  • Retract height: 0.125" from ‘Stock Top’
  • Clearance height: 0.125" from ‘Retract height’
    Fusion360 has defaults of 0.2" and 0.4" (respectably) which is excessive for Maslow with total 0.6" raise between G0 fast movement. If you have applied the Cheap fixes for z-axis slop on the Ridgid R22002 then the maximum raise is about 0.5" because the added bushing restricts max movement. If you use the Fusion defaults it will raise too high and possibly bind. This can stress the bushing glue joint, causing it to fail, and will cause stress on the height adjustment arm causing it to fail. Using these setting will avoid this.
    For each operation (contour, pocket, bore etc) set these height settings then right click on the input and select ‘Make default’. From this point forward this tool operation will use the reduced height settings so you do not have to change them again. You have to do this for each tool operation.
    This greatly speeds up cuts because z-axis movement is slow, reducing clearance height (compounded) to 0.25" from default 0.6" saves many minutes on z-axis movement.

Input requested
I have searched, high and low, but cannot find info on setting z-axis depth between multiple depth passes. Fusion360 will raise the bit to ‘Clearance height’ (0.25" in my settings) between each depth operations. This is a huge was of time as the bit should simply go down to next cutting depth. Right now it raises bit to 'Clearance height" every time which wastes a lot of time because z-axis movement is slow.

Does anyone know how to stop the gcode from raising up to ‘Clearance height’ between multiple depth passes? Right now the my gcode will raise the tool to +0.25" above stock, between each height operation, which is not necessary. It should respect last cut depth height and adjust the bit to go down from that point, rather than going up to ‘Clearance’ height.


There is a setting ‘keep tool down’ on the toolpath setting. last tab

I know i have to check it on 2D contour.


Thx. Will check that out.


This has my :+1: for getting bumped up somehow…how do we do that? This is great info!