Rotary Machining

This section is for useful tips and tricks for Aspire

Rotary Machining

Postby fwanek » Tue Jan 09, 2018 2:02 am

Hello All

I am working on a large piggy bank project 10” in diameter and 10” tall. My intention is to finish the O.D. using the rounding toolpath, which I’ve completed successfully. I’ve also included a cove top and bottom, as well as a pair of ½” spirals around the O.D. using the fluting toolpath. All of this seems to function as expected, however, there is such a disparity between the Y axis speed and the B axis speed, that I am ending up with a severe burn on the coves.

I am running the router as slow as I can (10,000 rpm). The rotary axis chuck is manufactured by Sherline ( and limited to something less than 3000rpm), with no visible means of adjusting its speed. I’ve no idea how fast it runs, but I’m guessing 3 rpm. (fast mode using the keyboard – machine control is much less ) My CNC is driven by Mach 3, and is a 3’ X 3’ machine manufactured by Velox CNC. I suspect that I’m well within the capability of the hardware, but cannot seem to overcome the slow speed difference between Y axis and rotary axis.

Can anyone suggest a fix for the speed difference???

Posts: 3
Joined: Sat Feb 07, 2015 11:15 pm
Model of CNC Machine: Velox 3' X 3'

Re: Rotary Machining

Postby PaulRowntree » Tue Jan 09, 2018 5:50 am

Frank, have you checked the maximum speed (and acceleration) that Mach3 is allowed to move each of the 3 axes?
Paul Rowntree
WarpDriver, StandingWave, Topo and gadgets available at
Vectric Wizard
Posts: 1671
Joined: Sun Oct 24, 2010 7:28 pm
Location: Guelph, Ontario
Model of CNC Machine: homebuilt 4'x2' (Mach3+G540)

Re: Rotary Machining

Postby Mike-S » Tue Jan 09, 2018 4:21 pm

Yeah, go into CONFIG/MOTOR TUNING and try increasing B axis speed.
User avatar
Vectric Wizard
Posts: 966
Joined: Mon Jun 13, 2011 6:45 am
Location: Hayesville, NC
Model of CNC Machine: Joe's Hybrid 4x4 (but 3x3)

Re: Rotary Machining

Postby ger21 » Tue Jan 09, 2018 5:10 pm

In Mach3:

Go to Config > Toolpath, and check the box that says use rotary axis for feedrate (something like that).

On the settings page, you need to enter the radius of your part for the appropriate rotary axis.
Note that you don't actually set the radius, but rather the Z zero location relative to the center of rotation.
If you set Z zero to the top of your part, then enter the part radius.
If you set Z zero to the center of rotation, enter .001 for the radius.

This should get your feedrates to compensate for the diameter.
Vectric Wizard
Posts: 967
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Rotary Machining

Postby Wod » Tue Jan 09, 2018 5:14 pm

First, make sure that the motor tuning for your rotary axis is optimized. On mine, the velocity is about 10 times higher than my X axis, and my acceleration is about 100 times higher than my X axis. Play around with these until your satisfied that it's running efficiently without loosing steps.

Under the General Configuration in Mach, make sure that the Angular Properties has a check mark in the box for your A axis is angular.

Under Toolpath Configuration choose your axis of rotation. One of mine has the A axis along the X and the other one has the A axis along the Y. Choose the one that is right for your setup. Put a check in the box for Use radius for feedrate. Put a check in the box for A Rotation enabled.

Under settings put your part diameter in the box for your rotary axis, probably A. When you run a different sized part, just put its diameter in and Mach will compensate.

You'll know that everyting is set up right when you go to the Program run page and the Radius Correct light beside the A axis is lit.

Hope this helps,
Posts: 5
Joined: Sat Feb 21, 2009 3:06 pm

Re: Rotary Machining

Postby fwanek » Fri Jan 12, 2018 9:43 pm

Thanks a bunch for the info - super good. This seems to be doing the trick for me. Once again - thank you very much for the informative response - appreciate your time and effort.
Posts: 3
Joined: Sat Feb 07, 2015 11:15 pm
Model of CNC Machine: Velox 3' X 3'

Return to Aspire - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 3 guests