I've been trying to cut a 13 TPI thread with MachTurn G76 and the pitch I'm getting is about 6% shorter than what I requested.  I'm running in metric mode so I use a P value of 1.954. While the thread is being cut the Feedrate DRO displays a value of 1.84 MM/REV instead of 1.95 and in when the thread is done the thread doesn't match a 13 TPI gage so I'm pretty sure the DRO is displaying what's actually happening. As far as I know there's no feedrate override in effect. I also tried a 20 TPI thread with a P of 1.27 and the DRO displays 1.20 MM/REV.

I don't know if this is related to the problem or not but although I've requested a spindle speed of 400 RPM the exact speed I'm getting is about 384 PRM which is about 4% slow. Mach does sync to the spindle so I don't think the speed difference is a problem.

I looked at code that's generated by the G76 macro and the G32 command is being passes a feed rate of 1.95 so the problem isn't in the macro.

FWIW I do have the "Use Spindle feedback in sync mode" box checked. Also my max feedrate is 1200 MM/MIN so I'm not trying to exceed that.

Can anyone think of what might be going wrong?

Thanks,
Drew

If you attach your xml I will take a look and see if I can find a problem.
Hood

Thanks Hood. The xml is attached.

Drew

Drew,
What version of Mach3 are you using?

Your spindle speed should be within at least 1% of what you command, actualy +- 1 rpm, the more accurate the better for threading, and no slow down of the spindle
while cutting the thread.

RICH

I'm not exactly sure of the version number but it was downloaded from Newfangledsolutions last week.

The problem with getting very accurate spindle speed is that I'm using a VFD and adjusting the analog output of the CNC4PC C11 interface board is pretty touchy. That and at low RPMs the VFD/motor combination isn't very stable. I was under the impression that with with a spindle index pulse Mach would adjust the feedrate to the spindle speed. With in reason of course.

According to the MachTurn_1.84 manual section 5.4.6.6, exact spindle speed is not likely to be important. Maybe tomorrow I'll try turning on the spindle Closed Loop Spindle PID control and see if I can tune it yo make things better.

Drew

You have your spindle pulley ratio set to 0.97 , set that to 1 and see how you go.

Hood

Drew,
Change the pulley ratio as Hood noted and let us know how it goes.

Do a scribe test to check threading results making mental note of the rpm fluctuation.
Spindle speed is important when threading.

You can find a lot of info on threading in "Threading on The Lathe" write-up which can be found in Members Doc's.
For the pitch use 4 decimal places. Note also that whatever value  you input if using the threading wizard Mach will use
what is input.

RICH

BTW,
Mach monitors the spindle speed during the cutting / threading of the material. If the rpm is not steady and fluctuates then it
tries to correct for it in the next thread pass. Thus the spindle speed control and thread correction can end up fighting each other. The recomendation is to set the rpm manualy.

Thanks Hood and Rich. That fixed it. But it does seem to imply that Mach thinks the Spindle Index is before the "pulleys". Kind of strange but Hey! as long as it's working!

I'll be sure to check out the "Threading on The Lathe" doc. Thanks or the pointer Rich.

Drew

That is what the ratio is for, say you have an encoder/index pulse on your motor but you have gearing from motor to spindle. That would mean the motor speed does not represent the actual spindle speed, this is why you set a ratio.
Mach can then work out what the actual spindle speed is from looking at the motor speed.
Hood

I guess that's one way to do it. However to me it seems odd to think of a motor index when everything is in terms of the spindle; spindle speed, spindle index, etc. The pulley on my machine's motor is 85% the size of the one on the spindle so I actually though that I should have had a value of .85 (or maybe 1/.85) for the pulley 1 ratio. But since my index is on the actual spindle that would have messed up the feed per rev. I'm able to setup my VFD to tale care of the .85 difference. Oh well, at least it's working now and I appreciate all the help.

Drew