Rotary Engraving Issue

[George Brown]

I am using my rotary lathe attached to my camaster cnc router using mach3. It is working out really well, but have a question. To get descent feed rates, ie. to get the rotary to turn at a reasonable rate, I have to set the feed rate at 2400 ipm. Cutting on an x-y plane, that would be rediculous, but with the rotary, that is the only way I can get it to turn fast enough. Is this normal, or am I missing something in my setup?

Thanks

[Wes Grass]

Are you actually engraving, or just test running the rotary? If the latter, the '2400' may be interpreted as degrees per minute. During actual cutting with the axis' synced it should work out right, assuming you've got the configuration set correctly for the diameter you're working on.

[George Brown]

I am actually cutting. For that type of job, I would be running at 100 inches/min, but if I set that, I can barely see the thing move it is so slow. Have to set it to 2400 to get a reasonable cutting speed. I think I have everything set right, the work is coming out correctly.

[Nicholas Bukky]

George I have a camaster as well with a rotary but I am running wincnc. I too run mine and program it at high feed rates sometimes up to 6k or 7k. Keep in mind it is running in degrees not the same as on the table top!! This is normal!!

Hope that helps!
Nic

[Gerry Grzadzinski]

Couple things.

1) Is the axis set up using steps/degree?

2) In Config >Toolpath, do you have Use Radius for Feedrate checked? If so, you need to enter the radius in the radius DRO on the settings page, IF, Z zero is on the surface of the part. If Z zero is the center of rotation, then enter .001 for the radius.

[Greg Holt]

The following is an explanation that I wrote a while ago on the "Use Radius for Feedrate" feature in Mach3

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


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

So what is 60 ipm on the linear axis (desired speed of the tool in the work), is 60 degrees per min for the rotary.

That 60 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 "Rotation Radius 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 Offset" 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 Offset" 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 Offset 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 Offset" 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 Offset" DRO when zero is the correct and desired value. Small enough to have no measurable effect on feedrate, but not zero.

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

The last two paragraphs no longer apply to the latest development version, but do apply to older versions.

Hope this is of some help.

Greg

[George Brown]

Thank you all for the good info. I missed the Rotation Offset Radius DRO. Thank you, very good explanation, that will give me the constant cut rate that I needed.

BTW, the camaster rotary is working out very well. With the stepper, I can cut all my rotary designs. I'm adapting it to be used for as a cnc lathe with the router as the cutter (replacing the stepper with a constant speed motor), and by replacing the whole rotary bed with a vertical plane, I can use it to bore holes into the edge of panels. Not bad, three uses for one attachment!