## A axis speed

Topics related to wrapped rotary machining in Aspire or VCarve Pro
RichardV48
Vectric Apprentice
Posts: 53
Joined: Fri May 01, 2009 5:05 pm

### A axis speed

I have a question about a lathe I converted for cnc. I created a rounding tool path for a piece of 2 inch square stock 6 3/4 long using a 1/4 end mill to cut it. The problem I ran into was that once I started running the file the rotary axis rotates at one degree per second, took 54 minutes to round the part. When it rapid moves it is much faster. Is there a way to control the speed of the rotary axis or does the software control it based on the feed rate of the X asis? I'm new to rotary but having watched some Youtube videos they seem to run much faster when they cut.
Thanks,
Richard

4DThinker
Vectric Wizard
Posts: 1416
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

### Re: A axis speed

Unfortunately your A axis is converting/using inches per minute as degrees per minute. Mine does the same thing. To overcome this I edit any toolpaths that will become A tool paths (rotational) to a much higher value, say 5000. You can do some math to know how high to get an equivalent feed speed on your A axis. If your cylinder is 2" diameter, the circumference is 2pi or 6.28 inches. If you desire a feed speed of 100ipm then you'll want 100/6.28 or 15.9 revolutions every minute. 360 (degrees in one revolution) times 15.9 equals 5,730. Put in a feed speed of 5,730ipm for any tool path that becomes A axis moves for a 100ipm performance.

4D

NormanAlbert
Vectric Wizard
Posts: 394
Joined: Wed Apr 01, 2009 12:15 am
Location: Dunnellon, Florida

### Re: A axis speed

To add to what's been said so far, don't forget as the diameter gets bigger the loads on the rotary drive get higher. If missed steps become an issue, that's probably where the problem is. Norm

IslaWW
Vectric Wizard
Posts: 1308
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: The Ultimate Woodworking Machine
Location: Marquette, MI, USA

### Re: A axis speed

Richard...
Which control software are you using? Most have a way to provide a proper rotary feedrate based on XY feeds. ShopBot and WinCNC via some PostP math and Mach from an onboard calculator.

In any event, the simple formula for rotary feeds (in degrees) that match surface feed rates (in inches per minute) is: 115 * [XY feed in ipm] / diameter
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

RichardV48
Vectric Apprentice
Posts: 53
Joined: Fri May 01, 2009 5:05 pm

### Re: A axis speed

Thanks for the responses.
When you talk about editing the tool path, what exactly are you editing? I went back and looked at the rounding tool path but I dont see any feed rates for the rotary. I had the motor tuning for the rotary axis set at 5000. I have doubled it and notice no difference in the speed of the rotary axis. The only time I see a slight improvement is by increasing the X feed rate but it is barely noticeable.
This is a home made conversion, so to get really good quality I am stuck running at slower feed rates.

I am using Mach for the controller.

Thanks again for the feedback.
Richard

TReischl
Vectric Wizard
Posts: 3821
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

### Re: A axis speed

If you are using mach. Search through this forum and you will find information on how to set up mach. Trust me, you are not stuck with slow feedrates.
"If you see a good fight, get in it." Dr. Vernon Jones

TReischl
Vectric Wizard
Posts: 3821
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

### Re: A axis speed

Find the. "Use radius for feedrate" setting in mach.
"If you see a good fight, get in it." Dr. Vernon Jones

RichardV48
Vectric Apprentice
Posts: 53
Joined: Fri May 01, 2009 5:05 pm

### Re: A axis speed

Thanks, I will check that out.

Richard

RichardV48
Vectric Apprentice
Posts: 53
Joined: Fri May 01, 2009 5:05 pm

### Re: A axis speed

I found the problem! When the code for the rounding tool path was generated a G94 code was inserted. This is a feed per minute mode. I changed it to G95 which is a feed per revolution mode and the A moves as it should. I went back and looked at the options for a rounding tool path and did not see where you can select the G95. G94 must be a default.

dealguy11
Vectric Wizard
Posts: 1663
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA
Contact:

### Re: A axis speed

The advice above regarding an option in Mach to use radius for feed rate is the way to go. I don't use Mach any more, but when I did and that option was selected I didn't have to mess with G94 vs G95 issues. There is another parameter in Mach to automatically convert from feed rate to radial rate given a specific diameter of the part that you enter in Mach. It's been a couple of years since I used it, but look for it - it's there.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com