Getting started with LinuxCNC and a lathe

[MTNGUN]

Hmmm, I haven't used G95 yet so I may not be able to help with this.

I presume it would go something like this?:

G95 G01 X# Z# F0.002

Here is the documentation for G95, such as it is: G95 Gcode. It doesn't offer much advice other than to mention that "motion.spindle-speed-in" needs to be connected.

If it is like G76 (threading), it may need to be told that the spindle is turned on (M3) before it will work.

Also, many of the G95 examples found online include an "S" command. I'm not sure if that is required?

I searched for "G95" on the LinuxCNC forum and didn't find much. Apparently it is not commonly used.

Should I be trying to use G95 or is there a better way to do this?

Well, when in doubt use a G01. If you figure out your G95 let us know how you did it.

[bhowden]

Hmmm, I haven't used G95 yet so I may not be able to help with this.

Well, when in doubt use a G01. If you figure out your G95 let us know how you did it.

G01 works fine now but I am pretty sure that it is supposed to be independent of spindle speed. All the docs I could find indicate that it is a general purpose move with feed specified in inches (or mm) per minute so it would move at the same speed regardless of spindle speed (which is what it seems to do with my setup) but then so does G95 so clearly I am missing something.

Perhaps I should be trying something like G76 but that seems more complicated than a straight move. I am also still a bit confused about the difference between the speed set with an M3 command and the actual speed reported by the spindle index sensor. I would hope that the feed is calculated using the feed back from the actual spindle speed but then why would you even need the M3 command.

Brian

[djc]

...Here is the documentation for G95, such as it is: G95 Gcode... If it is like G76 (threading), it may need to be told that the spindle is turned on (M3) before it will work.

I think you are correct here. It is important to understand the difference between modal and non-modal G-codes (see for example http://emc.sourceforge.net/Handbook/node65.html).

G95 shouldn't move anything in and of itself. Any movement you are seeing is because of a previous G01 in the file, that is still active. G95 just sets up a method (mode) of movement. For G95, the mode is inches per spindle revolution, as opposed to 'normal' movement which is inches per time period. G76 is a special case of G95 where the inches per revolution is additionally coordinated (indexed) with spindle position.

Think of it in a similar way to the code for coolant; you can G01 with coolant on; you can G01 with coolant off. You cannot and should not cause movement just by turning coolant on or off.

[MTNGUN]

I would hope that the feed is calculated using the feed back from the actual spindle speed but then why would you even need the M3 command. Brian

All I know is that G76 (threading) will not work without first doing an M3 to tell the machine that the spindle is on. This is true even if your spindle on/off is manual rather than controlled by the software.

G01 works fine now but I am pretty sure that it is supposed to be independent of spindle speed.

That depends on what mode the machine is in. In G94 mode a G01 should move in inches per minute:
G94 G01 X# Z# F# ; moves F inches per minute

In G95 mode G01 is supposed to move in inches per rev:
G95 G01 X# Z# F# ; moves F inches per rev

As DJC pointed out, G94 and G95 are not movement commands, they are modes.

[MTNGUN]

Update: curiosity got the best of me so I just now fired up a lathe and tried G95.

Using these steps:
-- machine activated and spindle spinning
-- G95
-- M03
-- G01 Z# F0.005

That resulted in the error "Cannot feed with zero spindle speed in feed per rev mode" even though the spindle *WAS* spinning.

So I tried again with an "S" Command:
-- G95
-- M03
-- S450 G01 Z# F0.005

And voila' ..... it worked ! And if I used the VFD to change the spindle velocity in mid-cut, the Z velocity would automatically increase or decrease to maintain the feed per rev.

That doesn't answer all your questions but it should clear up the mystery of G95.

[bhowden]

As DJC pointed out, G94 and G95 are not movement commands, they are modes.

Ah, the light goes on! Classic case of trying to fit all available data and advice into a preconceived notion. I did the G95 first as a separate command and then the G1. Now I get something like "Feed not valid with spindle stopped" and was about to start whining again when I remembered the rest of the advice you guys have been trying to give me. I tried again with a M3 S200 command and all is right with the world. The G1 command now works and the feed is proportional to the spindle speed.

Thanks again for the all the patience and help.

Brian