[Shotout]

Was wondering if anyone could give me some help with ridgid tapping. When I asked my instructor, he just grumbled about Haas' not being worth a dang at it. Can I set a peck tapping increment and what formula do you use to figure spindle speed. Erring on the side of caution I was going with the lower end speeds 100-150rpm and the taps where breaking on me. I'm mostly through tapping with a spiral point tap and work everything from plastics to 316ss. Any help would be greatly appreciated.
Thanks
Scott

[JPMach]

Small taps work better if the spindle is in high gear. You can either use a speed in that range or force the spindle to run in high gear. In low gear it takes a long time for the spindle to reverse where as in high gear it is almost instant.

I regularly tap 1/4-20 holes in aluminum with a form tap at 2500 rpm, even though the book says you should stay below 2000, I haven't broke one of those yet. I have run 5/16-18 at 1500 rpm also with no problems. I think when I tapped 316 SS 1/2-13 I was running around 300 rpm, I had a few of those break but it was more due to the material then anything. I had one break because the tap sliped out of the collet and when the machined moved to the next hole the tap was still in the last one.

To rigid peck tap you need to make sure that a setting is turned on that allows for repeat rigid tap. I have not done any peck tapping yet but many people say it works just fine.

JP

[Geof]

Peck tap works just fine on Haas; we use it on both lathes and mills. You do need to make sure that Repeat Rigid Tapping is turned on in Parameters.

We standardize on 1000 rpm because that makes it easy to calculate the feed and just repeat the G84 line with the different Z depths.

For faster retraction you can change Setting 130 or put a J value in the G84 line; J2 for us would retract at 2000 rpm. This saves fractions of a second and overheats the spindle braking resistor so it is hardly worth it.

[Shotout]

Thanks for the info. It is very much appreciated

[diggityds]

On a haas theres also some mechanical issues that can greatly effect your rigid tapping no matter how much you adjust your speeds and feeds. Theres a rigid tap belt that runs off the encoder to a pulley located on the gearbox. If that belt is in anyway damaged or loose it will throw off your spindle speed since rigid tapping follows the z travel encoder and the spindle speed encoder. Doesnt hurt to check that if all else fails. Good luck.

[shawncnelson]

I've tapped many holes on Haas machines. On a VF0 and VF4, tap sizes from 5/8 to #2 never had any problems. Also, there's no need to program a high spindle speed(1000+rpm). With the machines acceleration, you never actually reach higher rpm. Did a job once tapping 72 #10 holes(through 1/2 AL) , as an experiment, I changed the programmed rpm from 2000 to 600 and it changed the cycle time by ZERO. Not that having that S2500 is a bad thing, just never attained.

[Geof]

...... there's no need to program a high spindle speed(1000+rpm).

One reason to use exactly 1000 rpm; makes calculating the feedrate dead easy. 100 is too slow and 10000 is too fast.

[JPMach]

I've tried that too but on mine I got reduced time with the higher speeds. But then again maybe that is just because I have the 2 speed gear head, I can see that without a gear head it would not make much differnce. With the machine in low gear the motor is spinning close to top speed at 1000 rpm and does take some time to reverse, but in high gear and 1500 rpm the motor is spinning fairly slow and can reverse on a dime. If look in the manual it suggest using high gear on machines with two speed heads.

And yes on a short depth hole the 2500 is never attained but I regularly tap 1/4-20 to 1 inch depth and it reaches 2500 about 2/3 way through. I also tap 5/16-18 at 1800 rpm and can probably go faster yet and see reduced cycle time as it reaches speed quite early on.

Not sure but the difference may also be that my machine is fairly new and may have higher acc/dec rates on the spindle.

JP

[HuFlungDung]

JP,

How late model is your machine?

My '96 model actually runs the spindle 'open loop', which means that the machine does not really electronically cam the spindle to the Z axis motion, at least I cannot imagine how it could. The encoder index must give the start signal, and everything repeats after that. Mine works fine for repeat rigid tapping, I do not have a problem with breaking taps, and I tap down to #0-80 quite regularly. I use the theoretical tapping feedrate at the commanded spindle speed.

Having said that, it may bear looking at your actual spindle rpm. It should be very close to what you commanded, mine is out something like 5 to 10 rpm at tapping speed. It was out a bit more than that, and there is a bit of a tuning parameter on the drive which can be adjusted to bring the actual spindle speed a bit closer to the commanded speed.

I tap at only 500 rpm typically, because I'm tapping a lot of blind holes most of the time, and I want to stop fairly accurately at depth.

[Geof]

......I tap at only 500 rpm typically, because I'm tapping a lot of blind holes most of the time, and I want to stop fairly accurately at depth.

Try using a J value; go in at 500 and then use J4 to come out at 2000.

[JPMach]

HU: my machine is 12/2004. Who knows they may have changed something in 04 cause mine is one of the new ones without the hydraulic counterweight, just a bigger Z motor.
Yes for blind holes you have to go slower to have good depth control, but like Geof says use the J values to come out faster. I know in the book it says you can't tap faster than 2000 but I only read that after running 50 1/4-20 holes at 2500 without any problem, probably can't go any faster though.

my actual speed is within like 2-3 at those speeds @10000 it's off by like 6 rpm

JP

[HuFlungDung]

Try using a J value; go in at 500 and then use J4 to come out at 2000.

My control software is too old to have that feature. I looked for it

[ajl6549]

I regularly tap 1/4-20 holes in aluminum with a form tap at 2500 rpm, even though the book says you should stay below 2000, I haven't broke one of those yet. I have run 5/16-18 at 1500 rpm also with no problems.
JP

Does your machine acctually reach 1500 - 2000 rpm before reversing? In my exp. I've yet to see one reach those speeds unless the hole was quite deep.
Just curious.

A.J.L.

[JPMach]

like I said 1/4-20 at 1 inch depth it reaches 2500 probably 2/3 way through, 5/16-18 through .750" at 1800 rpm it reaches that probably half to 2/3 through. Of course for taps I generally start at a plane of +0.100" just to make sure that the Z axis is going as well, something I was taught for cnc lathes that I guess just carried through.

JP

[HuFlungDung]

Have you tried a longer ramp up distance? It seems to me that a lathe will give an imperfect thread if the axis is not up to full speed before it touches the work, and usually, the spindle is already running.

On a mill, I would wonder if the same principle would apply, that the spindle must be at speed before the tap has made some full threads in the part. The tap is the weak link so it fails in protest. At 500 rpm, I believe my machine is at speed nearly instantly.