## Mach3 settings

Topics related to wrapped rotary machining in Aspire or VCarve Pro

### Mach3 settings

I am trying to finish my a axis and can't figure out the steps per in the motor tuning screen.the motors have 2000 steps per revalution and I am using a 10:1 gear box so would that would make it 200 steps , but since it is 360 degrees should should the steps be 200 for a full turn or the motor or should I set it to .55 for the 1.8 degrees.
I hope this makes sense I am so confused I can't even explain this.
its just the mach 3 settings.

Thanks
mike1966
Vectric Craftsman

Posts: 101
Joined: Mon Jan 23, 2012 12:35 am
Model of CNC Machine: shopmade 5axis

### Re: Mach3 settings

You have a 200 step per rev motor. 1.8 degrees. I assume that is right.

Multiply that by whatever "micro steps" your stepper driver is set at. Lets assume ten micro steps for example.

200 x 10 = 2000 steps per motor revolution.

A 10 to 1 gearbox reduction. so 2000 x 10 = 20,000 steps per axis revolution.

Divide that by 360 to give steps per degree. 20,000 / 360 = 55.55555 Enter this number in Mach3 "steps per unit" for A axis.

Again, this is assuming some things. Use the appropriate numbers in the above calculations and all will be sweet.

Greolt
Greolt
Vectric Wizard

Posts: 880
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia
Model of CNC Machine: 900 x 750 2hp Mach3 Router & others

### Re: Mach3 settings

Thanks, I'll tried that and couldn't get it to work right it would go super slow read on the forum about the toolpath setting and rotational dro on settings page,I will try setting those and change the steps back to 55.555

Thanks
mike1966
Vectric Craftsman

Posts: 101
Joined: Mon Jan 23, 2012 12:35 am
Model of CNC Machine: shopmade 5axis

### Re: Mach3 settings

Slow is another issue.

First and foremost get the steps per unit correct and never touch it again.

When you command a 1 degree move, that is exactly what it must move.

Next comes an understanding of feedrate issues when using a mixture of linear and rotary movement.

Here is a copy of an explanation I wrote some time ago.

===========================================================================

All axis move in units per min. With a rotary axis those units are degrees.

So what is 120 ipm on the linear axis (desired speed of the tool in the work), is 120 degrees per min for the rotary.

That 120 degrees per min angular feedrate will make the tool move through the work at a speed dependant on the distance the tool is away from the centre of rotation. (in your case, very slowly)

So Mach has a feature to compensate the rotary axis feedrate, to accommodate differing radius that the tool is cutting at.

It is activated via the Toolpath Setup menu. Check "Use Radius for Feedrate" All the other settings in this box are to do with the toolpath display window.

On the Settings page there are three DROs labelled "Rotation Radius". IMO they would be better labelled "Origin Offset"

They are to tell Mach the distance that the relevant axis origin (Z in this case), is offset from the centre of rotation. (A axis in this case)

So if you are machining on the outer surface of a 10 unit diameter job and Z axis origin (zero) is set on that outer surface, then the correct value for the "Rotation Radius" DRO is 5. The distance that Z origin is OFFSET from centre of rotation.

If, on the other hand, the Z axis origin is at the centre of rotation (my preferred method for most jobs) then the correct value for "Rotation Radius" DRO is zero. The distance that Z origin is OFFSET from centre of rotation is zero.

Mach takes the Z axis DRO value and the "Rotation Radius" DRO value and adds them together to ascertain at what radius the tool is cutting at any one time. Then compensates the angular feedrate to have the tool move through the material at the desired speed.

Maximum velocity as set in motor tuning is honoured, so that will always be the upper feedrate limit.

Now there is one little "Gotcha". A zero value in the "Rotation Radius" DRO will automatically disable the entire feedrate compensation feature. This is a known bug.

The workaround for this, is to use a very small value (eg. 0.001) in the "Rotation Radius" DRO when zero is the correct and desired value. Small enough to have no measurable effect on feedrate, but not zero.

=================================================================================

Hope this helps

Greolt
Greolt
Vectric Wizard

Posts: 880
Joined: Fri Sep 21, 2007 1:44 pm
Location: Australia
Model of CNC Machine: 900 x 750 2hp Mach3 Router & others

### Re: Mach3 settings

You don't want to use deg, you indexer will move like a snail. Use radian 6.283 = one revolution. If you need a pp for radian send me a request.
Don
Dclifton2
Vectric Wizard

Posts: 320
Joined: Sat Feb 13, 2010 9:41 pm
Location: Port Orange Fl.
Model of CNC Machine: home built shopbot clone. CNC lathe