[Delw]

I got about 150 m6x1 holes to tap in some 17-4. having problems with the pull out as it breaks a tooth or 2.

I went to peck tapping and now I am at .025 depth per peck slow slow. its in a blind hole however they is no chip build up. tried spiral flute spiral tip and regular plug taps
what taps you guys recommend for 17-4?
I also tried pecking at .150 depth and .100 depth but it all breaks on the reverse( pull out) at least it makes the taps easy to remove.

my rpm is 50 rpm and the feed is 1.968 aything faster ( like 100 rpms with the correct adjusted feed rate)and I snap them going in on the first 2 threads.
I am sure its a tap issue as all my other tapping works fines.

tapping 17-4 is worse than 304ss.


Delw

[Geof]

What are you using for lubricant? Stainless is a real pain to tap and standard coolants are often not up to it. You may need to put in an M00 so you can squirt some really good tapping lubricant into the holes.

[Delw]

I use q cut its pretty thick, but to be on the safe side I ran a few holes with oil made no difference.
Just for the heck of it I hand tapped a hole and I get the same thing hand tapping.
The worse tap was a brubaker(sp) there brittle to begin with.
I got like 8 boxs of different configuration 6mmx1 but of course they are all not made for ss or crappy materials.
I had some emug(sp) taps for inconel but there all 1/4-20s so they wouldnt work.
time to go shopping in the AM.

Delw

[GermanTec]

Have a look at the setting 130. Change it to 1 and try it again.

[fizzissist]

I was having some issues tapping 0-80 blind holes in 304...called the tech guy at Emuge and was more than pleasantly surprised at the help.

[Matt@RFR]

I was instructed to use form taps on 304 and that solved all my problems with broken taps. Either that, or thread milling would probably be the safest route to take on difficult materials.

Have you double checked your actual hole size? Just a couple days ago I had a drill go undersized by .001" for a 6-32 thread and instantly broke the tap. I only had those drills on hand so I remounted it until it had some runout and made a larger hole. Then it was .0015" oversize and no more broken taps.

[Delw]

Have a look at the setting 130. Change it to 1 and try it again.

Ok would you or someone mind explaining it to me on what that option exactly does? please
I understand it brings the tap out faster or slower? if thats the case then now I understand why the option needs to be set.
I have a hard time understanding it mainly cause I very rarely have done rigid tapping untill we got this vf2ss last year.

I was having some issues tapping 0-80 blind holes in 304...called the tech guy at Emuge and was more than pleasantly surprised at the help.

They didnt have emuge taps but got some Japanese one specifically for this. so far so good.

I was instructed to use form taps on 304 and that solved all my problems with broken taps. Either that, or thread milling would probably be the safest route to take on difficult materials.

Have you double checked your actual hole size? Just a couple days ago I had a drill go undersized by .001" for a 6-32 thread and instantly broke the tap. I only had those drills on hand so I remounted it until it had some runout and made a larger hole. Then it was .0015" oversize and no more broken taps.

Matt yes I checked I am right at the mean dia. I am thinking of opening it up a tad with a reamer,
however so far so good on the taps. even cut the pecks down to .05 depth still left the rpm at 50.

I almost bought a thread mill today, havent used them and I dont want to scrap parts, as far as the roll tap. to be honest I never thought about that, I mean I did but always assumed they would break in tough materials.

you have had good luck with them I take it on 304?


Delw

[Matt@RFR]

Setting 130 sets the retract speed of the tapping operation via a multiple. If you set it to 1, then the tap retracts at the same feed as it went in. If you set it to 2, then it retracts at double the feedrate. I usually have it set at 4 for aluminum, but I've never really played with it much to see how far one could take it.

I machine very little steels, mostly aluminum, but yeah, I had great luck switching to a form tap in 304. One tap made about 200 holes and went back in the drawer for the next job versus the same brand cut tap that only made it about 5 holes before breaking. Spindle load will be higher, but a non issue for the size you're doing. For reference, spindle load on a 1/2-13 form tap in 304 with a .4695" hole was right at 60% in an '07 VF-2ss.

You'll want to use some form of tapping fluid for form taps though. Anything but aluminum/magnesium and regular coolant aint going to cut it in my limited experience.

[Delw]

Setting 130 sets the retract speed of the tapping operation via a multiple. If you set it to 1, then the tap retracts at the same feed as it went in. If you set it to 2, then it retracts at double the feedrate. I usually have it set at 4 for aluminum, but I've never really played with it much to see how far one could take it.

I machine very little steels, mostly aluminum, but yeah, I had great luck switching to a form tap in 304. One tap made about 200 holes and went back in the drawer for the next job versus the same brand cut tap that only made it about 5 holes before breaking. Spindle load will be higher, but a non issue for the size you're doing. For reference, spindle load on a 1/2-13 form tap in 304 with a .4695" hole was right at 60% in an '07 VF-2ss.

You'll want to use some form of tapping fluid for form taps though. Anything but aluminum/magnesium and regular coolant aint going to cut it in my limited experience.

Matt
Thanks for that info I think mine is set to 3 or 4 it spins out pretty fast
I might try the form tapping later. I generally used it on alum only and have played on soft steel.


the tap made quite a few parts since I changed it to a good tap, but still hearing that crack made me nervious. so I opened the minor up .002 and it made all the difference in the world still .0015 under the max minor.
went from a 5mm minor (.1969 to a .199) all the difference meaning I dont hear that crack when it backs off.

Delw

[offsetxyz]

I would really suggest getting a single point thread mill. We just finished a job that had about 20 broken taps. We got a single point thread mill and it works great. We aleady use thread mills with multiple points for larger sizes all the time. I would program it to drop to the bottom thread and spiral out of the hole myself. Thread mill program apps can be found at several places where tools are sold online. I would work it on a test block until I knew I was doing it right and then go for it. Program it not online but allowing for tool diameter or you can have problems with the cdc engaging in the hole. Some cdc is fine but say .090 cdc in a .234 dia. hole is not so easy. The thread mill will cost you over $100 each.

[Delw]

xyz
I do tons of thread milling single point style almost every day, I prefer it, however I didnt have one that small( after my tapping issue I have a vauge thought about it) and there wasnt a good quality one in stock locally so it had to be ordered in. I dont order anything unless its through a local supplier I support the local guys the best I can. everytime I have ordered any type of tooling online out of state I have gotten burned.

btw so far one tap has done 80 thread holes so I am going to bump it up a notch and see what happens.

Delw

[jamesu229]

We tap 17-4 on a regular basis. Use the maximun diameter tap drill, castrol molydee tapping fluid, torque control tap holder, a quality slow spiral tap and run at 20sfpm in and 3x out . works every time.

[Machineit]

What most people do not know is that the deeper you tap or the thicker the material that you are tapping, the larger the drill you should use.

There is a chart in your Machinery's Handbook, I don't have my latest edition with me, so I can't give you the page. I have my antique 1943 edition and it does not have the chart.

Drill and tap charts are only good for about 1 diameter of thread. For example, the chart will call for .201" drill for a 1/4-20 tap at 75% full thread. But, this is only for about a 1/4 inch deep tapping. As you go to 1 1/2, 2, and 3 times the diameter of the tap, the hole to drill gets larger. If memory serves me correctly and it seldom does at my age, if you tap 3/4 inch deep with a 1/4-20 tap, the holes can be about .218" in diameter and still considered as 75% full thread. I will find the information in my latest book and post it.

I worked at a shop where they tapped a lot of stainless, mostly 304, and they always wanted these deep holes even if they were not necessary. People were breaking taps all of the time and I spent hours removing broken taps. When I printed out the minimum and maximum hole sizes for our most commonly used taps, the breakage was mostly eliminated.

I'll find it and post it today.

Mike

[Machineit]

OK, sorry I didn't get this posted yesterday as noted, but here it is.

My latest version of Machinery's Handbook is #23. Starting on page #1654 there is a chart of "Recommended Hole Size Limits Before Tapping Unified Threads"

It has them listed by Classes, 1B-2B and class 3B. 1B and 2B are in one column and 3B is under another column. The hole sizes are listed in four depths each, To and including 1/3 D, above 1/3 D to 2/3 D, 2/3 to 1 1/2D, and 1 1/2 to 3D. D=the tap size, such as 1/4 inch.

I'll list a couple of examples below of class 3B thread holes:

-----------To 1/3 D,--------above 1/3 to 2/3 D-------2/3 to 1 1/2D,-----1 1/2 to 3D
-
-------------Min Max-------------Min Max--------------Min Max---------Min Max

4-40-------.0849 .0894---------.0871 .0916 --------.0894 .0939-------.0902 .0947

1/4-20-----.1960 .2013---------.1986 .2040 --------.2013 .2067-------.2040 .2094

As you can see a 1/4-20 tap run in only .400 deep can use a .2094 hole and still be a legal class 3B. It is much easier to tap too.

Using the largest hole possible and also within class limits will make the job a lot easier. This is especially important in tough to tap materials and small taps. We did a lot of 4-40's in excess of .450 deep in stainless and going to the larger hole size saved a bunch of broke taps. Just 1 or 2 thousands makes a tremendous difference in ease of tapping.

Hope this helps you all out. I checked and the chart is changed by the formatting software, so I hope it can be understood. I fixed it the best I could.

Perhaps this should be posted as a separate post to inform more people. None of the machinists I worked with knew this, they only used the standard chart for tapping. So every hole for a 1/4-20 was the #7 drill, no matter how deep it was.

Cheers Mike

[colton_m]

I had the same problem with 1/4 - 20 holes in 304ss.

The only way I could get it to stop snapping on the pull-out was to peck tap using propor tapping fluid at about 20SFM.

I also increased the tap drill size so it was only a 69% thread.
Would your application allow for a larger drill?

[nfrees114]

Thanks a Ton for this information!!!! I'm new to the tapping and I'm one of those, whatever the chart says kinda guys. Still Learning.... So with this chart, what is the depth of pass for tapping this stuff? Is it a one shot deal or a peck tapping?

Thanks!!

OK, sorry I didn't get this posted yesterday as noted, but here it is.

My latest version of Machinery's Handbook is #23. Starting on page #1654 there is a chart of "Recommended Hole Size Limits Before Tapping Unified Threads"

It has them listed by Classes, 1B-2B and class 3B. 1B and 2B are in one column and 3B is under another column. The hole sizes are listed in four depths each, To and including 1/3 D, above 1/3 D to 2/3 D, 2/3 to 1 1/2D, and 1 1/2 to 3D. D=the tap size, such as 1/4 inch.

I'll list a couple of examples below of class 3B thread holes:

-----------To 1/3 D,--------above 1/3 to 2/3 D-------2/3 to 1 1/2D,-----1 1/2 to 3D
-
-------------Min Max-------------Min Max--------------Min Max---------Min Max

4-40-------.0849 .0894---------.0871 .0916 --------.0894 .0939-------.0902 .0947

1/4-20-----.1960 .2013---------.1986 .2040 --------.2013 .2067-------.2040 .2094

As you can see a 1/4-20 tap run in only .400 deep can use a .2094 hole and still be a legal class 3B. It is much easier to tap too.

Using the largest hole possible and also within class limits will make the job a lot easier. This is especially important in tough to tap materials and small taps. We did a lot of 4-40's in excess of .450 deep in stainless and going to the larger hole size saved a bunch of broke taps. Just 1 or 2 thousands makes a tremendous difference in ease of tapping.

Hope this helps you all out. I checked and the chart is changed by the formatting software, so I hope it can be understood. I fixed it the best I could.

Perhaps this should be posted as a separate post to inform more people. None of the machinists I worked with knew this, they only used the standard chart for tapping. So every hole for a 1/4-20 was the #7 drill, no matter how deep it was.

Cheers Mike

[Machineit]

Thanks a Ton for this information!!!! I'm new to the tapping and I'm one of those, whatever the chart says kinda guys. Still Learning.... So with this chart, what is the depth of pass for tapping this stuff? Is it a one shot deal or a peck tapping?

Thanks!!

This was only meant to show how we often use the wrong hole size for the depth we are tapping. The hole size itself has nothing to do with peck tapping or single pass. That said, it is so much easier to run a tap down one inch in the larger hole.

When you use a larger, but still correct hole size, you only loose the very small tips of the threaded hole. Kind of like sanding a couple of thousands off of the threads of a machine screw, it would make no difference in the strength of the bolt. But, it drastically reduces the force needed to turn the tap and reduces binding.

On a very deep hole, the tap will actually swell slightly as it heats up, not much, but enough that the tap will swell slightly in the hole and so the top of the hole can bind. When the tap swells even .0002 the part of the hole already tapped will still be the original size as tapped and will begin to bind the tap.

I'm rambling but, using a .201 hole for a 1/4-20 tap going down an inch and a quarter is just asking for trouble that we don't need.

Thanks---Mike

[Seltzer Customs]

Try a compression tapping head. Where I work, we cut a lot of 303/304 and particularly on the job I’m working on. We have 4- 1/4"-20 through holes in 304 we've chosen to stop breaking cut taps and use forming taps. Unfortunately we don’t have a compression head in a 40taper so we use the Bridgeport. Even at 70%, with a brand new tap, rigid tapping doesn’t end well for us. An A drill will let the tap go through but not without bringing the finished size hole to .215...... But I believe as long as there’s adequate tapping compound and a compression head to lessen the torq shock when forming the thread, good preperation is good results. Machine coolant just doesn’t seem to do the trick…

Ran a job a week ago 60 ss304 parts, one through hole each, #1 .228 drill drilled spot on every time, compression head in the bridgy running prob 200+rpm, pink tapping compound(can’t think of name), didn’t break one tap, not one squealed in or out.

[rharter52]

Thread Milling is the way to go.Carmex makes a great thread mill.