Retract clearance with rigid tapping

[Vern Smith]

On this and other forums I've seen recommendations to start the rigid tap cycle a couple of hundred thou above the hole to give the spindle time to get up to speed. I've been wondering about this because the spindle has no problem handling the speed changes at the bottom of the hole so why would it need to "get up to speed" at the top?

The running start would probably be a good idea where the tap size is getting close to the peak spindle torque available but I can't see where it makes any difference in normal circumstances. I've always set .2 to be on the safe side but is it necessary?

Vern

[Geof]

I do this as well and recently I also realised it was illogical for the reason you give; but it is habit and I keep on doing it.

Your 'running start' for large taps does have some merit I think but I was thinking about the spindle torque on most of the Haas machines at 1000rpm which is the speed at which I tap. I think it is well above 30 or 40 lb-ft and when I imagine putting this type of torque on a tap I am in the 3/4" NC region or larger.

[Vern Smith]

Geof,

I have a job that entails drilling and tapping a couple thousand holes, fifty plus at a time. The extra .150 up and down a couple of times with peck tapping really starts to add up. As you say, I don't think 8 mm - 1.25 should be a big challenge for my 10 Haaspower.

Vern

[Geof]

When you are into the thousands yes seconds add up, especially in drilling. Just recently I clued into using the full range of options in G83 to do the first peck deeper than all the succeeding ones and this way you can shave seconds off a drill cycle. Also make sure the Setting Exact stop X Y is turned off provided you are not working with obstructions. This starts the Z moving from your start plane down to the R plane before the X and Y position has settled.

[Vern Smith]

Thanks for the tips. I'm a couple months into G code so I was not aware of the differential peck availability. I'm half afraid to turn off the exact stop because I might forget to turn it back on. I guess this would be a place for macros, if I had them.

Vern

[big_mak]

Vern,

I've tapped with the Retract setting at 0.05" and had no issues. Tapping @ 3000 RPM hasn't been an issue yet form me either(In Ally Granted) Tapped A36 Mild steel plated 1/2"-13 @600 RPM No Problem.

One Trick for I use for tapping is to change the feed to Feed Per Rev, then your F value = the tap pitch, and if you want to change your RPM, you only need to change the S value, and the feed stays the same(you don't need to recalculate the feed). Just remember to turn it back to Feed per Minute, once all your tapping is done.

That may help as you want to try and tweek your tapping speeds as you get into your production run, with a lower chance of errors!

[Vern Smith]

Mac,

Good ideas. I've been meaning to run some timed tests with high RPM and smaller taps, quarter inch and less. I have a feeling that the time saving will not be as much as one would think. If you watch your spindle speed during tapping it spends very little time at the set tapping speed. Most of the time its decelerating or accelerating. Now if you go one inch deep in one shot with a 10-32 you will probably see some serious time saving. You run that test, I don't have enough nerve.


Neat trick changing from IPM to IPR. The next neat trick is remembering to change back.

Vern

[big_mak]

Vern,

What size are you tapping in what material? One thing that can save you time in the tapping cycle is to make sure, you don't have an M03 at the beginning of the cycle. YOu can go Roll Form if the material allows it. Even Solid Carbide Roll form.

Let us at it!!!!!

[Geof]

Originally Posted by Vern Smith ......Neat trick changing from IPM to IPR. The next neat trick is remembering to change back. Vern

That is why I use 1000rpm; my old brain can handle the challenge of moving the decimal point 3 spaces for the feed rate and it doesn't have to worry about remembering anything to change back.

[big_mak]

Vern,

U use OneCNC? It's in my post processor!!!!!! IT changes back all by itself.

[dcoupar]

I think the .200 clearance is a holdover from the old days of tension-compression holders where you wanted to be sure the tap had time to "spring" out of the hole before XY took off at a blazing 200IPM to the next hole. I haven't used that kind of clearance since my first time rigid tapping. Like Geof says... "It is a habit" for some folks.

[Vern Smith]

Mak,


I do use One CNC, if I had not started with OneCNC I would still be trying to figure out how to drill a bolt circle. I purchased the software a month or so before the machine was delivered in February. That way I had something for the machine to do immediately and learned the machine operation from there.

As far a G code is concerned I thought I had discovered the Higgs bosen when I successfully constructed a 3 peck tapping cycle. I guess what you are telling me is that you modify OneCNC's threads per inch to inches per revolution through your post processor. Give me a week or so and I might get that to work.

I noticed that OneCNC outputs a M03 with all my tapping cycles. As Geof pointed out to me in an earlier thread, the G84 and G74 cycles are built around spindle rotation so I assume the M03 is redundant; however, how does it slow down the process? Does it cause the spindle to start, stop, and then restart when the G84-74 line initiates?

90% of my tapping is in 6061 and 2024. I use form taps most of the time although I've heard that they are not as good as cut threads in aluminum. That's probably a good subject for another thread.

Vern