I need to make some cams, for a project, and did the code in BobCAM-CAM, ver 24. using their 4th Axis Wrapping. The code looks fine, when you verify it, in BobCAD, but when I try to run it using Mach3, on a Taig 4 axis mill, the feed very move, with Feed set at 30 in/min.
 This is the frist time I have used the 4th Axis.

 Code
G90 G54 X.5837 Y 0.
G01 Z.4151 F 4.843
X.3279 A186.382 F30.0

 First two lines work fine, but X,A line, motor moves very slowly.
 If I do the X, and A on different lines speed is good, but can not cut the part, that way.
 Does any one have any idea of what is wrong?
Ken K

You do not have the 4th axis linked for feed rate coordination. As you ave it set it only moves at teh current feedrate in DEGs per minute not INCH per minute.

GOTO Config/Toolpaths

Then look at Rotations, select the axis of rotation (normally X), Select Rotations enabled, then select USE radius for feedrate

NOW go to the Settings page. Top right under Rotational radius and set the part's radius (diameter/2).

NOW Mach3 will correct the 4th axis feedrate (up to the top speed of the A xis) .

(;-) TP

 Thank you very much, for your help. It worked
 Ken K

What Terry said is correct.  Just need to add;

The DRO would be better labelled "Origin Offset"  (or something like that)

If you have the Z origin set at the outer circumference of the part, then enter the radius.

If you have the Z origin at the centre of rotation, then the correct DRO setting would be zero. (zero offset)

Whatever the Z origin is offset from the centre of rotation, is the correct value.

Mach adds this setting to whatever the Z DRO is, to determine what the Z axis feedrate compensation should be, at any given time.

IF you set it to ZERO it turns OFF the function.

Just a thought, (;-) TP

IF you set it to ZERO it turns OFF the function.

I thought that bug had been fixed.

I have a brain running that automatically puts a very small value in if zero is entered, so that is why I no longer notice it.

I have the same problem only my axis of rotation is X and the 4th is "C" on the screen (not the standard Mach screen) i did everything suggested above by BR549 and nothing changed. I played with the diameter as well and the speed didn't appear to change although I didnt put a Tach on it. It works but it's very slow, it's absolutely working in degrees rather than surface speed. I'm running the latest version of Mach. Thanks for any suggestions.

I am not sure whether or not the "rotary axis feedrate compensation" feature works on C axis.

I do know that only A axis rotations are able to be represented in the toolpath view.  Not B or C.

Suggest you try designating the rotary as A axis and see if that makes a difference.

Thanks for the Reply Greolt, I had suspected that and changed my ports and pins for the "C" axis to the "A"  and changed it in the general config but it wouldn't jog from the screen buttons. At that point I just switched it back, I guess I should have tried the G code anyway.  Does this mean  I will have to do a screen MOD which I haven't done before. Is there any way to switch it in the .XML file?

............... changed my ports and pins for the "C" axis to the "A"  and changed it in the general config but it wouldn't jog from the screen buttons.

  Does this mean  I will have to do a screen MOD which I haven't done before. Is there any way to switch it in the .XML file?

Are you using the standard screen for Mach3?

If so the jog buttons on the fly out screen (press tab), operate X Y Z and A. 

If this is not the case on yours, then someone must have edited it for the 4+ and 4- to jog C axis rather than A.

It is a trivial matter to change the behaviour of these buttons with a screen editor.  I recommend MachScreen.

On the other hand if you meant that the keyboard hot keys are what you are using, then these can be altered with menu "System Hotkeys"

Greolt