Can you tap too Slow?

PegroProX440 · Nov 27, 2019

I do not do production work, occasionally a 30 part order or something along those lines. Most everything is one-offs. I have had good luck with my current process tapping holes but was wondering if I am leaving a lot on the table. (I know if its not broken don't fix it..... but I love hearing what others have to say)

I program every tap I use from say #6 to 5/8 at 100 rpm. Its easy to figure out the pitch/feedrate that way.
The Machine I am currently using is a Mazak 510C. Even though I do not particularly like the machine it taps very well. I understand 100 rpm is super slow..... but is there benefit to going faster in my situation.

Will taps last longer if run in the appropriate speed range? Can my machine keep up?

camhead420 · Nov 27, 2019

I program for a small shop, like you no big lots. That is how i program to. One of our guy's even cut's that in half for tapping smaller than #10-24.
We did have a job running some aluminum casting's on a production job, we doubled the tap feed and speed for that, 3/8 -16 at 320rpm @ 20ipm.

DMF_TomB · Nov 27, 2019

PegroProX440 said:
I do not do production work, occasionally a 30 part order or something along those lines. Most everything is one-offs. I have had good luck with my current process tapping holes but was wondering if I am leaving a lot on the table. (I know if its not broken don't fix it..... but I love hearing what others have to say)

I program every tap I use from say #6 to 5/8 at 100 rpm. Its easy to figure out the pitch/feedrate that way.
The Machine I am currently using is a Mazak 510C. Even though I do not particularly like the machine it taps very well. I understand 100 rpm is super slow..... but is there benefit to going faster in my situation.

Will taps last longer if run in the appropriate speed range? Can my machine keep up?

.
1) hand tapping is slower usually 20 to 60 rpm obviously it works ok
.
2) some machines when at tap depth slide usually Z stops but spindle might keep turning. this extra turning the tap wants to pull out of tap holder which is not good if each hole it pulls out further and further. a spring extension compression holder allows the tap to extend out. when coming out of hole you often see it snap back suddenly what it was extended out for.
.
3) end of year if you tap say 3000 holes and break say 3 taps which took 15 hours to either get tap out or remake part. calculate time and material loss dealing with broken tap. if tapping faster saves 2 seconds a hole or 6000 seconds or 1.7 hours per year versus time and material loss from broken taps. ..... do the math
1.7 hours versus 15 hours
.
a car can often go 110 mph but if you drive that fast and crash car 3 times a year do you really save any time or money cause of car crashes ?

Mtndew · Nov 27, 2019

Yes you can tap too slow.
I've never understood why some people use the same rpm for all tap sizes. That's like using the same rpm when turning a 10" diameter piece of steel on a lathe down to 1/2" diameter.

DMF_TomB · Nov 27, 2019

hahahaha
.
tapping slow going to cause big problems. hahahaha
.
must have been mistaken hand tapping slow for over 4 decades and no problems. got to be cnc people who never do any field machining and manual machining

as9100d · Nov 27, 2019

Mtndew said:
Yes you can tap too slow.
I've never understood why some people use the same rpm for all tap sizes. That's like using the same rpm when turning a 10" diameter piece of steel on a lathe down to 1/2" diameter.

2000 rpm for every size!

Sent from my Pixel 3 using Tapatalk

DMF_TomB · Nov 27, 2019

obviously never used machine that has trouble with sync on slide travel to spindle turning
.
extra tap depth and tap pull out can cause problems. big tap over 3/4" usually resistance to turning helps slow spindle. little tap has so low turning resistance i have seen tap turn extra til it hits hole bottom or shank of tap hits cause went too deep breaking tap
.
even if breaking taps happens only 3 times a year it usually causes a lot of time and material loss

KC3KNM · Nov 27, 2019

I'm pretty conservative when tapping. That said, I don't run production and normally only have enough stock on hand for one go at a part with short turnaround time. Even if a tapping cycle takes 30 minutes longer than it could have with more aggressive parameters I'm making out.

As previously stated, it's all dependent on what you're doing. Too slow is relative, in my uneducated opinion.

Mtndew · Nov 27, 2019

DMF_TomB said:
hahahaha
.
tapping slow going to cause big problems. hahahaha
.
must have been mistaken hand tapping slow for over 4 decades and no problems. got to be cnc people who never do any field machining and manual machining

Does your IQ drop on a daily basis or what?

gustafson · Nov 27, 2019

If you are running 6-32 threads .5 deep with .1 clearance you are spending like 12 seconds tapping each hole. 8 holes on a part and you are watching it for 3 minutes, not including traverse

I run at least 1200 rpm, its over in 15 seconds or something

If it isn't a problem for you it isn't a problem for me, but I think I might fall asleep

It's not so much that you need to go faster, but don't you have something else to do?

as9100d · Nov 27, 2019

For small taps, buy a big Kaiser tapping head and never worry about it again. We would tap that #6 at 2000rpm and never look back.

Sent from my Pixel 3 using Tapatalk

NAST555 · Nov 27, 2019

I also run pretty conservatively because I am in the same boat most of the time... Not big production but every so often might get, say, 500 holes on a run. I generally tap from about M6 - M16 but I don't run the same RPS's. It is all material dependent. The M6's I run in the 500 RPM range and M12 from 300-400.

Having said that I had to tap some M24's a while back. One of my machines has a gearbox so it could handle it no problem (don't judge... I held the tap in a sidelock holder and it worked beautifully). I started REAL SLOW... Like in the 40 RPM range if I remember properly. I bumped it up and it actually tapped loads better. I think I landed up in the 200RPM range.

eaglemike · Nov 27, 2019

Yes, you can tap too slow. One important part is the torque range of the machine. I've also experienced problems going to slow when the torque range should not be a factor. I suspect it's something to do with the material flow when form tapping. Lubrication makes a big difference - see the other thread about tapping in 303.

gustafson · Nov 27, 2019

eaglemike said:
Yes, you can tap too slow. One important part is the torque range of the machine.

That is an important point that I had not pondered right up front. once you get over 1/4 roll taps there can be quite a bit of torque involved.

rcs60 · Nov 27, 2019

I think that with one off's the op should do what works for him
if tapping takes 5 sec or .5 sec there isn't much difference in the cost of the part
the biggest factor when tapping is what is the machine/ process capable
does the machine have rigid tapping
what are the limits of the rigid tapping
what are the limits to the tap being used and how it is used (hand tap/ spiral point/ bottom tap/ high spiral / or form taps)
material being tapped
so with out this information it would be hard to say if the op is leaving anything on the table

i have tapped 10-24 form taps in aluminum at 800 rpm because that is all the machine would allow
also tapped 10-32 in 12L14 at 4000 rpm in a production part (about 10000 holes)

Job Shopper TN · Nov 27, 2019

I generally tap most things at 20 SFM. Honestly it can be done faster. Now, yes, you can tap as slow as you want, a la hand tapping. But, sorta like drilling etc., you may be rubbing more than cutting, a negative for tool life, and tool life is probably more important with a tap than anything, broken taps mean rework or scrap. Yuck.

But it depends on your machine. I will say, even with rigid tapping CNC machines, it seems that things do go better with a holder that has some play in it, like the newer Techniks Synchro chucks, or the old school tension/compression.

garyhlucas · Nov 27, 2019

One issue I can see with larger taps going slow is that a VFD spindle with say a 6,000 rpm spindle tapping at 100 rpm is well into the speed reduction where the torque really falls off. So the results and strain on the machine may be much better at say 500 rpm. As others mentioned the high torque needed to tap will help brake the tap to a stop going in, and you need higher torque initially on backing out because you have static friction and chip breaking to overcome.

G00 Proto · Nov 27, 2019

I'm one of those idiots that taps everything at one RPM... 500 RPM, nearly every size, nearly every material. [I do make exception for production and parts with hundreds of tapped holes, and I think about SFM for exotic metals]. I could be more efficient and have faster tapping cycles, but I memorized all of the tap feeds in IPM years ago based on 500 RPM. This has saved me from having to do hard math

and I can glance at the G84 line of code and instantly see that the feed is correct. As a matter of fact, if I went back in time, I would have the young me get a tattoo on my arm for Imperial taps; drill size, clearance size, and feed at 500 RPM. Not only would that have saved me a million looks at the wall charts, but I strongly believe it would have helped me pick up thousands of good looking women that saw the wisdom in such a tattoo.

eaglemike · Nov 27, 2019

For metric threads, when I had a Haas, I tapped everything as a multiple of 254 rpm, usually 1016 or 1524, because I'm lazy. Feed per Revolution didn't come out to a perfect number in an inch machine, to it was easier to keep IPM. Worked really well. I did have fewer broken taps above 750 rpm, and only slowed down when I was tapping 8mm or 10mm in stainless.
As an official Brother fanboi, I should mention that tapping on a Brother is easy, no matter what RPM is best for the material. The G77 cycle uses J for inch threads, as in J20 would be 20 threads per inch. Then I and the value for metric, as in I1.25 for 1.25mm pitch. I love form tapping 6061 at 4K-6K rpm on these machines. For a guy that started in a shop that still had a few lineshaft machines, this is truly amazing.

706jim · Nov 27, 2019

Most of my programming was done at a school. To simplify calculations for imperial taps I just multiplied TPI by 10 for the rpm. So 10-24 would rotate at 240rpm and 10ipm feed. 3/4-10 100rpm 10ipm feed etc. And the machine used had a low gear 50 taper spindle so tons of torque. But I'm aware that new machines work at speeds in a completely different universe.

Can you tap too Slow?

Hot Rolled

Cast Iron

Diamond

Diamond

Diamond

Stainless

Diamond

Plastic

Diamond

Diamond

Stainless

Stainless

Stainless

Diamond

Plastic

Cast Iron

Stainless

Hot Rolled

Stainless

Titanium

Similar threads