[tko829]

I recently (Couple of months ago) upgraded to Pathpilot on my PCNC 1100. I had used the Mach3 control to do some turning work, holding material in the spindle and turning tools in the vise. Now, I have a job to run for a customer that requires the same process. However, since I have switched to Pathpilot, this was an untested area for me. Now I can't get the G95 (Feed/Rev) command to function. When the machine gets to the point where it is supposed to begin cutting, it just sits there. The book says it should work. Has anyone used their Pathpilot control on a mill as a lathe successfully? I'm pulling my hair out, and I need it to work!

Thanks for any help!

Btw, has anyone used the G96 (Constant Surface Speed) command on their mill? It looks promising, but I need the G95 to work first.

[adamvs]

The mill wasn't really intended to be a vertical lathe, so I doubt the mill supports CSS or G95. You may have to just fix it[the gcode] by hand. Just leave the line at Sxxx M3. No G95.

[tko829]

I realize it wasn't intended to be a lathe, but it has been done by several others. There are some pretty cool Youtube videos showing what they have done. I have done it myself, back when I was running Mach3.

The reason I want G95 (feed per rev) to work is because it is in the Manual for Pathpilot provided by Tormach. I am simply asking for what the manufacturer says will work. If it doesn't work, it would be nice of them to note that in the manual instead of explaining how to use it!

The CSS is a separate item, but again something that is in the manual.

[tmarks11]

I will bet you that it works when PP is in lathe mode (it would be ridiculous if it didn't). Wonder if this is a bug, that G95 is disabled when in mill mode.

[tko829]

I think it is a bug. That, or a very serious typo! I submitted a bug report, but was hoping that someone would have an answer so that I could get up and running quickly. I'm certain I can get away with programming in inches per rev, it's just a little frustrating to see your machine not function like the manual says it should!

[adamvs]

I think it is a bug. That, or a very serious typo! I submitted a bug report, but was hoping that someone would have an answer so that I could get up and running quickly.

I stand corrected, so my mill post produces a G94, I can see what because on a mill it's really about SFM and chip load, and since the number of teeth is unknown feed per rev is kind of meaningless. I'm working on supporting the mill as a lathe in a post for Fusion, so yes this and CSS would be nice to have. It's pretty clear that the mill version and the lathe version are two separate code bodies just by the fact that some 'shortcut' features implemented in one aren't implemented in the other. I'll submit this as a bug also, more bug submissions might get their attention.

[TurboStep]

I will bet you that it works when PP is in lathe mode (it would be ridiculous if it didn't). Wonder if this is a bug, that G95 is disabled when in mill mode.

I bet you that it works when PP is in Mill mode too! I just tried it - works as I expect
Step

[tko829]

I bet you that it works when PP is in Mill mode too! I just tried it - works as I expect
Step

So your PP mill will feed using G95? How do you do it?

Sent from my Venue 8 3830 using Tapatalk

[adamvs]

So your PP mill will feed using G95? How do you do it?

Sent from my Venue 8 3830 using Tapatalk

I just tried it on my 1100 running PP 1.9.4 - it abruptly stopped at the first G95. Also come to think of G96 is probably ( just guessing ) not available until they get an encoder kit for the mill.

[TurboStep]

So your PP mill will feed using G95? How do you do it?

First the good news, both G95 and G96 work with PP.
Then the bad news, I got mixed up between them. G96 will work on a Tormach out of the box but G95 requires a spindle encoder to sync with the spindle. What you're experiencing is PP waiting for the spindle feedback - which obviously won't come without the encoder.
Quote from the cnclinux pages "G95 requires that motion.spindle-speed-in to be connected."
If I cover my encoder sensors it just sits there as you reported.
Sorry about my initial confusion.
Step

Edit: I checked the latest PCNC 1100 manual and it is listed as a "valid" command. Either this is just a copy/paste error carried over from the lathe docu or there is something interesting in the works... but no, I haven't found anything in the code yet

[tmarks11]

This is too funny. Works on TS machine because he has added on an encoder. Guess the OP needs to buy some more hardware...

Looking at the Mach3 (Aug 2013) and the PP version (Oct 2015) of the Tormach manual, the wording for the G95 command is exactly the same, so that isn't really a clue of a future product improvement.

[TurboStep]

... , so that isn't really a clue of a future product improvement.

Oh well, never mind, perhaps they'll get there sooner or later.
Step

[tko829]

This is too funny. Works on TS machine because he has added on an encoder. Guess the OP needs to buy some more hardware...

Looking at the Mach3 (Aug 2013) and the PP version (Oct 2015) of the Tormach manual, the wording for the G95 command is exactly the same, so that isn't really a clue of a future product improvement.

What is frustrating is with the exact same hardware, I was able to run G95 in Mach3, no encoder required. I could see a need for an encoder to get G96 working. But feed per rev should work on a programmed spindle speed.

[adamvs]

Oh well, back to old school: multiply RPM by FPR and you have IPM.

[tko829]

Oh well, back to old school: multiply RPM by FPR and you have IPM.

Yeah, kind of a letdown, though.

[TurboStep]

What is frustrating is with the exact same hardware, I was able to run G95 in Mach3, no encoder required. I could see a need for an encoder to get G96 working. But feed per rev should work on a programmed spindle speed.

Actually with PP its the other way around. G96 works without an encoder and as you said you can get away with programming in inches per rev instead of G95, but I can't imagine an easy alternative to G96.
From what I understand the duality lathe only has an index pulse and PP simulates an encoder using a "modified encoder HAL component" so perhaps you could copy the HAL mod and get away with something simple like this: C3 - Index Pulse Card for just $26.
Step

[adamvs]

Also if all hammer on Tormach to come up with an encoder kit for the mill, that would also mean rigid tapping, which would be very nice!

[cncoperator]

Also if all hammer on Tormach to come up with an encoder kit for the mill, that would also mean rigid tapping, which would be very nice!

I'm pleased Tormach doesn't have rigid tapping and hope they don't add complexity to the machine. I find my tension compression head works well and don't see much reason to have something else to fail or add cost to the mill. Sold by Tormach:

Thread mills
Tension compression tapping head
Reversing tapping head

Please no rigid tapping since it adds another failure point and cost. Twenty years from now when I'm still using my Tormach and they have passed to the happy hunting ground I want a simple machine with a shot at being able to fix it myself.

[adamvs]

I'm pleased Tormach doesn't have rigid tapping and hope they don't add complexity to the machine. I find my tension compression head works well and don't see much reason to have something else to fail or add cost to the mill. Sold by Tormach:

Thread mills
Tension compression tapping head
Reversing tapping head

Please no rigid tapping since it adds another failure point and cost. Twenty years from now when I'm still using my Tormach and they have passed to the happy hunting ground I want a simple machine with a shot at being able to fix it myself.

Uhhh..ok.. but it would be an accessory to the mill, I would think, not built in.. otherwise they'd loose their market for, well, this accessory, plus tapping heads! It would also boost the base price of the mill which I doubt they would want. I think it would make a good add-on, rigid tapping works great on the lathe.

[TurboStep]

Please no rigid tapping since it adds another failure point and cost. Twenty years from now when I'm still using my Tormach and they have passed to the happy hunting ground I want a simple machine with a shot at being able to fix it myself.

Nobody ever forces you to upgrade!!!
Step