[cam1]

Hi:
I'm having problems with a tapping cycle on a 3 X VMC with a FAGOR 8055iA milling control. The tap keeps on pulling itself out of the holder on the retract part of a G84 cycle ( I think). I read the tapholder instructions, and made sure to use R=0 (floating tapping cycle). I have tried to use some dwell (K=200) and also tried reducing the feedrate to 49 IPM on Tapmatics advise. They say to reduce the feedrate by up to 5% on through hole tapping.

Material= 6061 T6 1/4 thick
Tap: 1/4-20 Spiral flute
tap drill=#7
RPM=1000
Feed= 50 IPM, also tried 47.5,48 and 49 IPM
Floating Tapholder=Tapamtic NS4 with a jacobs rubber collet sized for a .257 OD shank.
Cooloant= Flood semi synthetic

My gut tells me that I may be using up the float (.25 inch) when I get to the bottom of the hole, and the spindle may be continuing to rotate.(After all it only takes 5 revs to eat up .25 inch).
Then, when it retracts, I may have already used up my travel with the holder, so the tap has no choice but to be pulled out.

Not only am I pulling out the taps, but I'm beginning to pull out my hair on this one. I'm not blessed with alot of hair to begin with.

regards

[fuzzyracing1967]

I have no more hair becouse of problems like this! I have however had this same problem,what I found out was the tap was basicly screwing itself out of the holder(the collet couldn't hold it at the end point).Try cutting speed and feed in half,that worked for me.I use valenite holders on one of the older machines we have,and I hate that whole drift thing,you never know just where the tap will stop.

[cam1]

Thanks fuzzy, my tapholder is for unthreaded taps. It uses a rubber/metal collet and a pinch screw on the square to secure the tap.
Thanks for the information, I'll cut the speed in half. You would think that a VMC would be able to cut threads at 1000 RPM, but I guess the amount of drift I get when the spindle is slowing down, has used up all the float.
I wnet this route because I was having following error problems with the machine on the rigid tap cycle.

"For every solution there is a problem" has become my motto.

cheers

[little bubba]

Just a thought, if you were having problems with the rigid tapping, you may have a spindle encoder problem, and you may be running more RPMs than you or the machine thinks it is. Get one of those little hand held tachometers with the rubber tips and check it out, the little tachs are handy to have around for drill presses and manual machines also.

[cam1]

Thanks, good plan. I'll check this AM.
I'm also thinking that there must be a spindle decel parameter. At 1000 rev/min = 16.6 rev/s. I have 5 rev of axial float with 1/4-20 tap (.05" pitch). If the spindle take .3s to decel, I'll have eaten up the .25 of axial float with the holder. Now .3 of a second is not alot of margin....

regards

[cam1]

As I thought the G84 tapping cycle (non rigid ) runs open loop on the spindle (duhh), the spindle acceleration/deceleration parameters as set by the OEM were a bit loose, nevertheless in open loop mode ther is no spindle brake. The answer is to lower the speed of the spindle , or to tune the Z axis/spindle so that I can do rigid tapping.

thanks for the help

[dunnitagain]

cam1. since you have some experience with the spindle speed problem... I too have a Fagor 8055i on a knee mill. Every time we reverse the spindle, it only turns about 50rpm. Ive looked for every parameter in the manual, and the spindle drive manual and can't figure it out. If i swap the input leads on the spindle drive, it works just opposite. It reverses fast, and moves slow in forward. That tells me it is in the control somewere. But where? Also I can't find an encoder anywhere on the spindle. Where is yours attached? They retrofit company sold us the rigid taping option. But how can that be done with no encoder? Any help would be greatly appreciated .!!

[cam1]

Hi:
We have a vector drive spindle, and yes, you must have an encoder to do rigid tapping.The spindle RPM and Z feedrate must be exactly synchronized. As far as the spindle rpm is concerned, id look in the machine parameters/spindle to see if there is a variable there. The variables are really intuative ie (spindle_max rpm_ccw). First, do a backup of all parameters via USB or RS232. Then pull out a pen and pad, and make sure to record the parameter that you are trying to change. Then change the parameter, and reboot the control.If it made no change, go back and set it to the original value. If you are not comfortable doing this, Id recommend phoning Fagor for tech support.They have always been most helpful when we call for tech support.

regards

[JROM]

using a 1/4-20 tap you use this to setup feeds and speeds

1 devided by 20 = .05 times your spindle speed (300 rpms) = 15 IPM get it?

1 devided by the threads per inch times the spindle rpms is the corect way to program a tapping cycle.

[dunnitagain]

Thanks for the help! We called FAGOR today,and finally found the problem. It was 3 simple parameters. The spindle speed MAXGEAR1 through MAXGEAR4 must be set accurately. The value is how the control and drive scale the RPM. Next the voltage values in P37-P40 are how the control syncs the spindle speed. You can use the values,and a hand held Tach to accurately set the spindle speed, to the indicated control rpm. Lastly the voltage param for the spindle drive output must be set to both + . The control default set is one is + the other - . The yaskawa drive wants only a + POS value for speed control,on a three wire hook up. Thanks Again for your help.

[cam1]

Excellent: I'm always happy when someone grabs the bull by the horns, and gets the job done.

good work

regards