Does anyone have experience rigid tapping with a Cent6 controller? My mill is supposed to have this option, and I would like to learn more about. Am I understanding correctly that you can chuck a tap up in there using say an ER-32 collet and program tapping? If so, what would be the better to use cut taps or form taps?

Thanks for any information.

Yes you can put your tap in a collet. the type of tap depends on what you want to do. material blind hole thru.

if you have rigid tapping you will need to have tap collets, they will hold on to the square end of the tap.

form vs cut

6061AL form or cut
brass cut
copper form
anything cast cut
1018CR cut
most CR lead steels form or cut
tool steels cut or thread mill
SST cut or form

if you have to pound a blind hole into some material
that you can form tap its best to use one. If not you can use a spiral fluted cutting tap that will send the chips up the tap not down like other cutting taps.

hope that helps

feel free to ask more questions

I tap with collets all the time, just got to make sure there tight. BTW, rigid tap on a cent 6 is a G88. Todd

Thanks for the reply guys. I'll have a chance to play with with it tonight and see if my mill supports this feature. The original owner had a hodge-podge of add-ons and didn't go with the package upgrades. I'm hoping this is one of them.

I haven't done any rigid tapping on my Cent.6. I have on my Cent.5. I don't know how familiar you are with the conversational side of the controller but they make it very easy to figure it out. Some guys don't care for the conversational programming, but I do a lot of prototype molds, and sometimes nothing can touch the speed in which I can create the program. I also use regular collets. I would have to say if you can use a form tap that is the way to go, especially in a blind hole. No chips

I attempted to do some hard right tap cycles and no love. The table moves in X/Y but no movement in Z. After looking through the documentation that came with the mill, the previous owner had a sheet of G and M codes hand written and next to G88 there is "Hard Tap (Not Avail)"

So, it looks like I'm out of luck :(

Looks like this is a $1200 option currently. I don't know that I would do enough tapping to justify that much money. I could put that towards a dedicated tapping table.

Thanks for the help and quick replies.

James

Rigid tapping works in a standard collet I have even used a drill chuck

I will agree with you guys, Rigid tapping will work with standard collets but be careful with your RPMs. I will some times rigid tap at 8000 to 10000 RPM and at those RPMs you need tap collets.

8-10000 rpm?:eek: Whats the point of that? In what kind of mat'l?

some of our jobs are very high production 5000 to 10000 pcs. per order so if i can decrease run time at all its worth it. i have cut taped and form taped at 8-10000 rpm in AL, brass, and copper. keep in mind those were not very big taps (6-32 up to 5/16-18).

Does anyone know exactly what one gets for $1200 with the rigid tapping feature from Milltronics? I mean is there some hardware they add or are they simply turning on an option in the setup?

I cant understand why anyone would tap at 10000 RPM Itwould take longer to excell and decell than you could savr

bill that is not tru. try it if you can or dare. I will start .100 above the part and by the time the tap hits the part its 10000 rpm. This is done on your Brother TC-22 VMC, some VMC might not beable to handle this.

I bet if you taped a series of holes @ 10000 then did them again @ 5000 there would be very very little time difference.

The rigid tap option gets you a encoder and belt and cables.
You will then need to tell the control it has rigid tap.
what is the serial number of your machine I can tell you if it was buildt with rigid tap.

Ok, I've done a number of tapped holes without a glitch until today. I programmed 4 holes .500 deep at 1000rpm and the machine tapped 1.000 deep! Now I have a broken tap in a blind hole in a $600 piece! I changed the depth to .250 deep and it still tapped 1.000 deep! Then I changed the RPM to 500 rpm and it works as it should. What gives? What does the RPM have to do with the depth.

Here is the code generated in Surfcam:
O1
G90G80G40G17
T19M6
G0G54X-0.886Y-4.252
M3S1000
G43Z1.H19
M8
G88G98X-0.886Y-4.252Z-1.489R-0.889F0.05
X0.886
Y4.252
X-0.886
G80
M5M9
G32
G49M2

This is a VM24 and Centurion 6 controller.

Well, For starters on your G88 line your asking it to tap Z-1.489 deep. So the fact that it only went down to 1" is amazing. your R plane with an initial height of Z-.889 is blow Z, zero. So i hope that your part Zero is - 1." from mat'l top or you asked it to tap more than 2" deep. With -1.489 - -.889 that still is asking it to tap .6" deep. if mat'l top is Z "0" then you would wan't your G 88 line to read G88 G98 X, Y, Z-.5 R.1 F.05

Sorry for the confusion, that particular post was from a set of four holes in a pocket that was .989 deep. If that confuses you, then here is a post with the holes at Z zero:

O1
G90G80G40G17
T19M6
G0G54X-0.886Y-4.252
M3S1000
G43Z1.H19
M8
G88G98X-0.886Y-4.252Z-0.5R0.1F0.05
X0.886
Y4.252
X-0.886
G80
M5M9
G32
G49M2

Could someone try this on their machine and see if it goes one inch deep? Then change the rpm to 500 and see what happens.

I'm wondering if your spindle encoder is working properly. It shouldn't overun that much or at all. I've done a lot of tapping with a cent 6 and 7, never had a problem. I don't have one available right now.

Spindle speed does have a lot to do with it.
when in rigid tap the spindle is servoed to the axis. soo if the spindle is at a higher rpm it takes longer to stop, thus making spindle go deeper.
There is a parameter in the misc paramers for hard tap fudge factor. this controls when the spindle shuts off. So at higher rpms this number needs to be higher. It is set at 70 this is good to around 500 rpm depending on what spindle motor you have. You may want to set it to around 200 for 1000 rpm.

Mholden,

I tried your suggestion with little effect on the depth. At 1000rpm it still goes 1” deep. The fudge factor was original set at 0.000, I tried 70.000 and 200.000 with no change at 1000rpm. When I changed the rpm to 500rpm there was a slight difference in depth, .4 for 0.000 and 70 and .5 for 200.

I’m wondering about the spindle ramp up and down times (they are set at 4 sec. each). Could this effect rigid tapping?

4 secs maybe the problem.
set them to zero and try it.
how old of machine is this?

how old of machine is this?

The machine was built in 1999, VM24. The machines has been with us since it was new. The service guy changed the ramp time when it was installed for some reason I don't recall. What is the default supposed to be?

It would have been set to 3 and 3

OK, Setting it to zero works better and is closer to what I would expect. So my next question is: What does this setting do exactly? Is there a problem leaving it at zero? What would be the optimal settings for the ramp and fudge factor? Am I going to have to change this with every tap or does every one use just one speed for all taps?

Leaving at zero could cause a high amperage surge and fault out. I would set it 1/2 sec. - 1 sec. it's kind of harsh to ask a spindle to go from 0 - max in ZERO time.

i run fanuc at work but i figure tapping is tapping so i thought id put my input in. I have to rigid tap on the machine i use the most because we dont have a tapping head for it and i dont like it that much. i go through alot of taps if it the tap gets clogged your hosed but i only tap blind holes. im sure for through holes it would be fine. and i always just use regular collets and aroun 1000rpm usally 10000 could be intresting though haha

if you have rigid tapping you will need to have tap collets, they will hold on to the square end of the tap.



If you have rigid tapping you should be able to use a ER- style collet. dont use a jacobs chuck as they stuff the shank of the tap (if they slip) and make them un-usable with er style collets(if you have any).

ALSO:

I have never seen a tap collet let alone ever heard of one, i would like to see one though. maybe someone can post a picture of one?

http://www.rego-fix.com/screwmachine/taprigid.asp is the tap collets but I would use the rigid tap holder you can quickly chage taps if they break or get dull and hold the square shank.
http://www.techniksusa.com/metal/ttcartc.htm

The holder we have is like the one on this page:
http://www1.mscdirect.com/CGI/NNPDFF?PMPAGE=1604&PMITEM=00191569&PMCTLG=00

Only until recently we used a Drill press adapted for tapping but because of the size of some molds bases we decided to tap them in the Milltronics VMC. I’m trying to establish consistency in depth to prevent breakage because every hole is a blind hole in this business. Using 500rpm seems to give us the best results for now.

I have seen the RT feature over tap the depth many times in my cent6. However, this information is interesting, I will try some tests.

I always thought the z axis servo followed the spindle encoder. So if the spindle tries to get up to 1000 rpm and it takes too long to do so the control algorithm does not shut it down early (before it reaches commanded rpm).

I purchased the RT option and installed it myself. I do not remember any wiring harness except what came on the encoder. If you look in the head of the mill you will see there is a large timing belt pulley around the spindle. If you have RT it will have a belt around it and an encoder setting next to it. My encoder had a plug that connected right up to a plug that was hanging right over the area where the encoder goes.

Cheers
Dave