Toolpath configuration for 4th axis in Mach3

[m8298]

In one of the threads I read, Greolt mentioned to changing some settings in the Toolpath box in Mach 3. This was to enable Mach3 to calculate and adjust feed rate while performing 4th axis machining. I have a 4 axis table(X,Y,Z,A.) Can someone explain what the proper setting are? And do I only use these settings when cutting on the 4th axis?

[Greolt]

Here is something I wrote quite some time ago and have posted it various times over the years.

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

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 and is being addressed by Artsoft at this time. Hopefully it will be fixed soon.

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.

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

The issue mentioned in the last two paragraphs was fixed in a later version of Mach3. I don't remember when.

[m8298]

Hello Greg,

Thanks for the reply. Sorry for making you repeat it yet again. And for the record, you can take the credit as to why I got involved with this CNC hobby. I saw your stuff on YouTube and I was hooked.

So when you are talking about setting the rotation radius, is that what is called Stock Size in the Tool path Configuration window, or is there another window to open?

When you said: " Maximum velocity as set in motor tuning is honoured, so that will always be the upper feedrate limit." I take that to mean I don't need to change these settings only when using the 4th axis.

[fretsman68]

If you're using the standard screenset in Mach3, the rotational radius dro is set on the "Settings" page in Mach 3 in the top right of the page.

Hope that helps-
Dave

[Greolt]

So when you are talking about setting the rotation radius, .....................

I see by the pic you posted of the "Toolpath Configuration" window that you are using an older version of Mach3.

It is now called "Use Radius fo Feedrate" and "Rotation Radius"

Previously the rotary feedrate compensation feature had some serious bugs. This was fixed some years ago. With the "Gotcha" mentioned above fixed at a later date.

You had better update if you are going to be doing rotary work.

Greolt

[m8298]

You know, I just looked and you are right. I just updated. Now, I am using the 2010 screen set, any chance you can tell me where to find the Rotational Radius DRO? Or do I need to bounce over to the Mach forum?

[m8298]

Nevermind, I know where it is. Thanks guys.

[m8298]

OK, now I have a new problem. I don't know if its from updating Mach3, or what but now my homing routine doesn't work right. Arghh.?..

[Greolt]

If the 2010 screenset is new to you, then I suggest staying with what you have been using until you get it sorted.

Did you retain the profile from before or set up a new one?

Look at ports and pins to make sure inputs are assigned correctly. Diagnostics page is good to check manual activation of homing switches.

Check for modified or custom "Ref All" script.

Greolt

[m8298]

All of my macros stopped working.

[m8298]

All is working again. Not sure what happened, but I overwrote my macros with backup copies and I am working again. I've been using this screen set for a while and I really like it. Whew.

[Greolt]

Glad you got it sorted out.

Now get on with some rotary axis fun.