Poor Tool Life Tapping 0-80 Thread in 360 1/2 Hard Brass

[Nerdlinger]

I have very little personal experience with this particular process, but the guys I work with have been complaining about tapping this 0-80 hole because the tap life is so variable (i.e. 2,000 pcs vs 20 pcs). So here's the deal:

Machine - late 90's Hardinge GT Super Precision
Control - Fanuc 18T
Material - 5/32" diameter 360 1/2 hard brass
Part length - .075"
Tap - OSG Hy-Pro Tin coated 0-80 Form Tap
Tap Depth - .125"
Tap Drill - #55 all the way through the part plus a little deeper than the cutoff so the drill mark is still into the next part. (My chart says #54 for a form tap so maybe there's something there.)
Oil/Coolant - dry
Speed - S250
Code -

N25(0-80 TAP)
(FORM TAP)
(USE .052 #54 FOR NOGO AFTER TAP)
M9
G4U.3
M9
G4U1.
G10P0Z-.400
G97S250M3
T25
G0Z1.
G0X0
M36
G0Z.05

G99
G32Z-.120F.0125
M5
M4
G32Z.05F.011 (this has been changed too F.012 and F.0125 for some reason)
M9
G0Z1.
M37
T0
M1


(See attached pic) We're using one of those Tapmatic rigid tapping adaptors but maybe that's not enough float?

I called OSG and they said the RPMS were way too low. We stepped up to S750 and it broke on the first one. They also said we should use some coolant of some sort so we will try putting on a temporary M08 with oil prior to tapping but I am not all that hopeful.

Do you guys have any ideas? Sometimes there is a little flake of material on the tap after tapping...I wouldn't think should be there. Also, the guys I work with are confident that if they put a drop of tap magic on the tap before each part it will last forever.

So maybe just a M08G4U1M09 is all we need but I wanted to see if anyone saw anything else we are obviously doing wrong

Thank you!



Hey, you don't have to take pictures in landscape anymore!

 

[guest]

FWIW, I make a part from C360 that gets a 4-40 in the end. I run coolant, and run the tap pretty slow due to a tight thread depth spec.

Tap is a Balax bright form tap- no coating. Still on the first tap on that job, probably ran about 500 pieces all in.

 

[Mike1974]

We tap 0-80 all the time. Some aluminum, some brass (not sure of the brass properties or condition) with no issues. I have found that using a #55 will cause taps to break. You should use a #54... but we don't gage our threads, so I don't know if they would be in spec depending on your print callout (H3 or whatever..).

RPM = 1200
FEED = 15 ipm
FLOOD COOLANT = ON

Tapping to -.025 of the drill depth, ie drill .200dp, tap .175dp

We usually use Balax taps, uncoated, modified bottoming.

 

[pcasanova]

don't drill into the next part. If the drill point is visible in your next part and it walks just a bit, your drill is going to get pulled and not drill straight. then your tap doesn't have a chance.

 

[rcs60]

First thing i would do is to get a larger drill the #54 (.055 dia.) will give you about 60% thread the .052 drill (94% thread)is getting very close to 100% thread which is not good for form threading
a 1.35mm drill would give you about 70% thread if needed

G99
G32Z-.120F.0125
M5
M4
G32Z.05F.011 (this has been changed too F.012 and F.0125 for some reason)
M9
G0Z1.

from your code you are not rigid tapping this is a problem with the spindle and tap not being sync'ed up to make a good tapped hole with a Tapmatic rigid tapping adaptors
you will need a floating tap collet/ tool holder

using the G32
the feed into the part should be made at 80-90% of the pitch going in .011 IPR. Going out should be about 100-110% of the pitch .013 IPR
this would be to make sure you don't push the tap in damaging the threads and on the way out to keep it from crushing the thread on the way out


This is the threading cycle that i use for a 10-24 thread
M3S800
G0X0Z-.100
G32Z.300F.033
G32Z-.100F.0416M4(reverse spindle and z at the same time)
G4U.3(dwell to make sure the tap is out of the hole) (Machine and rpm dependent)
G0Z-.125

 

[Dan from Oakland]

Also, gage your hole size after drilling to make sure its the correct size- On small forming taps, a few thou can make a big difference

 

[DanASM]

don't drill into the next part. If the drill point is visible in your next part and it walks just a bit, your drill is going to get pulled and not drill straight. then your tap doesn't have a chance.

This.

Brass can "grab" the drill and pull it off center. When the drill goes into the next part and spots it a little it could be off center.

Use the correct drill for the form tap at 60%-70% threads.

Spot drill the part first. Then drill the hole, not past the cutoff. Tap looks a little slow (I dont have numbers here to tell you how fast).

Always use oil coolant when tapping. If your running dry then you need to have an operator there to dab the tap with tap magic or something for lubrication.

I run Brown and Sharpe screw machines with mobil met 766 neat cutting oil. It works fine tapping anything. I dont ever use tap magic but I hear it is excellent.

Edit: I just looked at my chart and it says 5043 or 4437 rpm for tapping in 360 brass.

 

[Nerdlinger]

Thank you, everyone, for the responses! It looks like we spot drill before drilling so I suspect the arguably-poor practice of drilling into the next part is not our problem....meaning I think the spot is rigid enough to not follow the drill mark left from the previous part. I am not sure “why” we drill into the next part.

I am interested in what rcs60 said about the G32/rigid tapmatic combo not being compatible. I, personally, have never used G32 and have always had the luxury of just putting an ER tap collet in a straight-shank holder or whatever and then using a rigid tapping cycle. I don’t even get the difference between a floating tap holder and that Tapmatic thing we use, but I get the feeling it is like a a somewhat-floating holder? But maybe not enough for our non-synchronized G32 cycle? I’ll have to look into this more, I think!

Thank you, again!

 

[DanASM]

Thank you, everyone, for the responses! It looks like we spot drill before drilling so I suspect the arguably-poor practice of drilling into the next part is not our problem....meaning I think the spot is rigid enough to not follow the drill mark left from the previous part. I am not sure “why” we drill into the next part.

I am interested in what rcs60 said about the G32/rigid tapmatic combo not being compatible. I, personally, have never used G32 and have always had the luxury of just putting an ER tap collet in a straight-shank holder or whatever and then using a rigid tapping cycle. I don’t even get the difference between a floating tap holder and that Tapmatic thing we use, but I get the feeling it is like a a somewhat-floating holder? But maybe not enough for our non-synchronized G32 cycle? I’ll have to look into this more, I think!

Thank you, again!

You may be drilling into the next part because the tap needs to go in a certain depth to get full threads. I did this recently and found I had to use a .156 cutoff tool instead of .90 or .125

This was to make sure the spot drill on the next part had a flat face to cut into and did not follow the previous drills hole.

This did make my material needs increase due to the wider cutoff tool.

You are on the right track now and should have all the info you need now. Good luck!

-Dan

 

[Nerdlinger]

from your code you are not rigid tapping this is a problem with the spindle and tap not being sync'ed up to make a good tapped hole with a Tapmatic rigid tapping adaptors
you will need a floating tap collet/ tool holder

using the G32
the feed into the part should be made at 80-90% of the pitch going in .011 IPR. Going out should be about 100-110% of the pitch .013 IPR
this would be to make sure you don't push the tap in damaging the threads and on the way out to keep it from crushing the thread on the way out


This is the threading cycle that i use for a 10-24 thread
M3S800
G0X0Z-.100
G32Z.300F.033
G32Z-.100F.0416M4(reverse spindle and z at the same time)
G4U.3(dwell to make sure the tap is out of the hole) (Machine and rpm dependent)
G0Z-.125

I have always had the luxury of tapping on CNC machines that have “rigid tapping.” This machine is the only one we own that does not have it. I suppose I never really appreciated what goes into syncing up the various axes. (I thought IPR was IPR but I guess it’s not that straight-forward!) So it seems like the adaptor we are using is closer to a straight up collet chuck than a floating holder and any variation in “actual” IPR is screwing up our parts. Soooooo I got a tension/compression holder on order and will feed in a little slow and out a little fast. I will report back but am very hopeful! Thank you!!

 

[DanASM]

I have always had the luxury of tapping on CNC machines that have “rigid tapping.” This machine is the only one we own that does not have it. I suppose I never really appreciated what goes into syncing up the various axes. (I thought IPR was IPR but I guess it’s not that straight-forward!) So it seems like the adaptor we are using is closer to a straight up collet chuck than a floating holder and any variation in “actual” IPR is screwing up our parts. Soooooo I got a tension/compression holder on order and will feed in a little slow and out a little fast. I will report back but am very hopeful! Thank you!!

I have always had the luxury of using floating holders with my machines. I know how to run them very well. You shouldnt have any problems if you get a floating holder. It sounds like you have the rest all figured out now.

Good luck and keep us updated with results

 

[guest]

...I don’t even get the difference between a floating tap holder and that Tapmatic thing we use, but I get the feeling it is like a a somewhat-floating holder?

I don't have rigid tapping on my lathe. I use a G32 cycle and a Tapmatic NC-1. It's a tension/compression/releasing tapping head.

Yours is different than mine, and I don't know how it works. I can't read it clearly, but in your pic it looks like that one is designed for #2 or M2 and larger?

Reason is- form taps don't self-start, and the hard start on the tapping head has to be firm enough for the tap to start. But not so firm that it snaps the tap, rather than extending past the detent on reversal.

When I run the #4 tap on mine, I back way off the hard start. When I run a 1/2-13, I crank it back down- that tap is a lot harder to get started.

Check the functionality of the tapping head. They do get dirty. Make sure it compresses and extends, and snaps back properly, but it's not too hard to push past the detent position. Gently blow it out and give it a little Boelube or similar. If it's too stiff to operate with the #0 tap, it's just like trying to rigid tap.

And did we mention to run some lube or coolant? Needs something so the tap doesn't just gall up in the hole...

 

[Ox]

I've never used M32 at all I don't think, but Shirley not for a tap, but if you are sometimes getting 2000 pcs - then it must work, but likely only at the slower rpm's, and this is going to be relevant to spindle reversal times possibly.

The holder that you have has just a little wiggle room, which is built for RIGID tapping, which you are trying to mimmik with G32, and apparently was having good luck before. I would start back at the slower speeds as the folks that rec'd faster speeds likely didn't understand that you're machine doesn't support RIGID and that you are using a crutch.

There seems to be aggreeance that you should bump your drill size up, and that might solve your issues.
Although I hate partial threads in formed holes!
They start poorly and have very low torque rating as there is nothing between the crests.
I'd try for that 1.35 that was mentioned.

#4 is the smallest that I have ever had anything to doo with, and I understand that form taps are tougher, but this is 360 brass eh?
Is a cut tap not an option?

Your code shows that there has been many edits, and that coolant has been used at least at some point in the past.
Maybe if you just burped the coolant on the tap quick?


--------------------

Think Snow Eh!
Ox

 

[Nerdlinger]

I can't read it clearly, but in your pic it looks like that one is designed for #2 or M2 and larger?

Reason is- form taps don't self-start, and the hard start on the tapping head has to be firm enough for the tap to start. But not so firm that it snaps the tap, rather than extending past the detent on reversal.

When I run the #4 tap on mine, I back way off the hard start. When I run a 1/2-13, I crank it back down- that tap is a lot harder to get started.

Check the functionality of the tapping head. They do get dirty. Make sure it compresses and extends, and snaps back properly, but it's not too hard to push past the detent position. Gently blow it out and give it a little Boelube or similar. If it's too stiff to operate with the #0 tap, it's just like trying to rigid tap.

You're right - the one we are currently using is designed to cushion rigid tapping cycles for #2-#10 so we are wrong on both the style and size of the tap (i.e. rigid tapping #2 vs unsynced tapping #0). I have a Tapmatic tension/compression holder that is appropriate for form tapping #0-80 in brass on order, so hopefully that cures what ails us! We are getting the "SM" version, so similar to yours but not quite as slick. So does the "hard start" feature keep the tool in position until a certain amount of force is applied and THEN it starts to float? Like you said - otherwise a form tap is liable to just spin on the entrance to the hole while the holder compresses?

Tried oil but no dice. In the meantime I might try running it at even slower speed, which might reduce the variation between spindle rotation and Z-axis feed. Thank you for your help!

Thank you!

 

[Nerdlinger]

I've never used M32 at all I don't think, but Shirley not for a tap, but if you are sometimes getting 2000 pcs - then it must work, but likely only at the slower rpm's, and this is going to be relevant to spindle reversal times possibly.

The holder that you have has just a little wiggle room, which is built for RIGID tapping, which you are trying to mimmik with G32, and apparently was having good luck before. I would start back at the slower speeds as the folks that rec'd faster speeds likely didn't understand that you're machine doesn't support RIGID and that you are using a crutch.

There seems to be aggreeance that you should bump your drill size up, and that might solve your issues.
Although I hate partial threads in formed holes!
They start poorly and have very low torque rating as there is nothing between the crests.
I'd try for that 1.35 that was mentioned.

#4 is the smallest that I have ever had anything to doo with, and I understand that form taps are tougher, but this is 360 brass eh?
Is a cut tap not an option?

Your code shows that there has been many edits, and that coolant has been used at least at some point in the past.
Maybe if you just burped the coolant on the tap quick?


--------------------

Think Snow Eh!
Ox

Thanks, Ox! I think you're right - running it slower might actually work better because I think it would minimize the variation between the spindle rotation and Z-axis feed so I'll probably try that while I wait for the tension/compression holder to come in. I'll have to look into the drill size...#55 is is a tad small but I wonder if we are off-center enough to make an effectively appropriately-sized hole. I'll have to look into if there is a reason we use form taps or of cut taps are fine. I thought there was a more-or-less consensus on using form taps for anything under like 1/4-20? Or maybe that doesn't apply to brass?

 

[guest]

...So does the "hard start" feature keep the tool in position until a certain amount of force is applied and THEN it starts to float? Like you said - otherwise a form tap is liable to just spin on the entrance to the hole while the holder compresses?

Yep, that's exactly how it works. It has a set screw in the shank, you can reach in from the end and adjust it to whatever tension you need. Pretty simple.

If that machine can't rigid tap, I will be surprised if slowing it down is going to help, but they're your taps!

 

[Nerdlinger]

I got the tension/compression holder installed. Even though I DO believe this is the proper tool to be using the taps were still breaking, so I changed to a #54 drill (you know, the one on the tap drill chart?) and so far so good! We're about 400 pcs in with no problems. I also added a brief splat of cutting oil on the tap so I'm not sure how much that is helping but I do believe the drill size was the problem. You can see in the attached picture how fully-formed the threads were with the smaller #55 drill. So that, combined with running dry, must have been the problem. For now I am keeping it at S250. I know I "should" go faster but for now I am happy that is just running with the "Repeat Mode" light blinking!

Thank you for the help, everyone!

 

[Delw]

I got the tension/compression holder installed. Even though I DO believe this is the proper tool to be using the taps were still breaking, so I changed to a #54 drill (you know, the one on the tap drill chart?) and so far so good! We're about 400 pcs in with no problems. I also added a brief splat of cutting oil on the tap so I'm not sure how much that is helping but I do believe the drill size was the problem. You can see in the attached picture how fully-formed the threads were with the smaller #55 drill. So that, combined with running dry, must have been the problem. For now I am keeping it at S250. I know I "should" go faster but for now I am happy that is just running with the "Repeat Mode" light blinking!

Thank you for the help, everyone!

View attachment 281448

Cool its working. thats not a bad looking thread for form tapping better than I thought it would look.

the minor for a 0-80 2b thread is max 0.0514 and min .0465

 

[precisionmetal]

I'm a bit late to the party, but I would personally use...

- correct size tap drill

- uncoated tap

- lubricating oil (not "cutting" oil)


A forming tap works much better with a bit of high-pressure lubricant (e.g. old-school 90-weight differential oil or something like STP). It's a forming process, not a cutting process.

 

[Nerdlinger]

the minor for a 0-80 2b thread is max 0.0514 and min .0465

We have a .052" no-go pin gage, so I guess that makes sense! Maybe I'll check with a variety of pins to see where we are at in the .0465-.0514 range and see if I need to get a slightly-different (metric) drill for next time. Thanks!