Mach3 change over help

[Rene2.5RS]

Hello All,

I need some help with some math in regards to changing a setup on a machine I am doing some work with. I work with a billiard cue maker and we have a 4 axis cnc miller, x,y,z,a. We are currently working on engraving designs in sections of the cue and we were told to swap the Y axis to the A axis. This worked well but now I need to reconfig the motor tuning in Mach3 to get the rotation to move in accurate increments (1 inch inputted, 1 inch traveled).

Want I want to do is create a new machining profile for engraving that will only use 3 axis, X, Z and Y set to the current A rotation stepper.

I will not be in front of the machine until tomorrow morning, but I do have the current motor tuning numbers if that will help. The X, Y, Z axis all are direct drive to lead screws. A is a worm drive to spin a straight gear. I am not sure if this will allow any you guys much smarter than me to figure out what to set the new Y motor tuning too.

Tuning # are as follows:
X and Y
Steps - 20,000
Vel - 18
Accel - 0.3
S. Pulse - 2
D. Pulse - 2

Z
Steps - 20,000
Vel - 18
Accel - 10
S. Pulse - 2
D. Pulse - 2

A
Steps - 350
Vel - 4285.8
Accel - 2000
S. Pulse - 2
D. Pulse - 2

I have attached pictures from the first test run. Everything worked, but the machine is not moving 1:1 as the program thinks. If more information is needed, please let me know what you need and I will have it tomorrow morning!

Thanks for any help you guys can provide.

-Rene

[ger21]

The problem you might run into, is that if the diameter changes, you'll need to change the motor tuning to match the diameter.

I'm assuming that your A axis is 350 steps/degree? If so, then you have 126,000 steps/revolution.

So your steps/inch would be (pi*diameter)/126,000.

You might find it easier to create 2D code, and use CNC Wrapper to right code to use your A axis. CNCWrapper - Home Page

[Rene2.5RS]

Bobcad v24 has a cylindrical stock milling feature which is what I tried first, but the problem I had was say for easy explanation when the code called for:
A30
A31
A35
A30

Everything would be fine until it had to go to a lower angle, it would spin completely 355º to go from line A35 to A30 rather then back turn 5º to get to A30

Not sure if that is just how Mach works or if there is a setting some where that can be changed

[ger21]

In General Config, uncheck "Rot 360 Rollover."

[Rene2.5RS]

OK, well that is good to know.

Only other thing I noticed was the rotational speed was following the same feed in the program which was painfully slow. I was cutting at 10ipm but as you can see from the listed motor tuning the A axis can go quite a bit faster. Is there a way to avoid having the A rotation follow the set feed rate in the program?

[Rene2.5RS]

OK, so I went back to try the actual A rotation and the problem I am having is there are points when the cutter drops into the work piece and then it just starts rotating, which would essentially cut a diagonal line in the work piece. I just purchased CNC Wrapper and hope it will provide better results...

[ger21]

I was cutting at 10ipm but as you can see from the listed motor tuning the A axis can go quite a bit faster. Is there a way to avoid having the A rotation follow the set feed rate in the program?

G1 moves should follow the feedrate, and G0 moves should be at rapid speed, which is defined in Motor Tuning.

and the problem I am having is there are points when the cutter drops into the work piece and then it just starts rotating, which would essentially cut a diagonal line in the work piece

The machine does what the g-code tells it to, which means your code is probably not correct.

[Rene2.5RS]

Gerry,

Big question for you. When trying to use CNC Wrapper, it keeps giving me an error message every time I load the g-code that arcs were found. Is there any way around this?

I should say, yes I went into options and unchecked the search for arcs. I am test running the code in a piece of work. I can see why it is searching for arcs. I am not sure what to do since there are so many arcs created when Bobcad auto gens the tool paths...

-Rene

[ger21]

You may need to get Bobcad to create code without arcs. Sorry, but I've never used BobCAD or the Wrapper, so can't help much more with that.

I know that a lot of CNC Wrapper users use Vectric software, which comes with posts that don't use arcs.

[Rene2.5RS]

Gerry,

Thanks for your help. CNC Wrapper looks like it will be very helpful once I get the arcs out of the posting. Bobcads internal post for doing the same thing doesn't use negative degrees which is why it will spin completely around to get to a called for degree.

Thanks for your help.

-Rene

Edit: Oh btw to get around the slow feeds, I just set to feed to 125 and all the other steppers stayed within there motor tuning max velocities