Help with tapping problems

[shorton2]

I have a small manual mill that I use with a tapmatic head to make some steel parts. My parts are initially cut for me, from 1/4" thick cold rolled material with a waterjet. I finish drill the holes to be tapped on the mill, then tap.

I use a non-sulpher cutting fluid manually applied to tap and hole. I've made hundreds of these things but the last 2 batches have given me a lot of trouble. Today while trying to figure out how to solve it, I've broken 4 taps.

I am drilling a 10-32 and a M6 hole.

I used a guide (my notes say from USCTI) to choose the drill size. I wanted a high percentage thread.

For the 10-32 I chose a #23 drill (0.154) which the guide said my probable hole size would be .1578. That would give a 79% thread.

I haven't changed anything in my process except obviously the steel may be slightly different from batch to batch, but it is cold rolled. I could have changed drill bits due to wear, not sure there, and the resulting finish hole could be different. I don't have a good way to gauge the true hole size. The #23 bit is a snug fit by hand.

I do not know what speed is best to use for this tap and material. I used to run at about 500-600rpm and didn't have problems, but as I was having problems lately, I tried to slow the speed. Initially that seemed to help, but then I broke some more taps.

Usually the tap wants to hang part way through the cut. Once it hangs, it's difficult to get out.

Can someone tell me what the correct rpm is for tapping a 10-32, and M6 holes, in 1/4" cold rolled should be?

And if my drill selection looks wrong, can someone offer any advise on the correct hole size to produce a high percentage thread that is close tolerance/tight?

Thanks,
Scott

 

[ornerynorsk]

Check your parts to make sure that they are, indeed, being waterjet cut and not laser cut. Laser cut will have hard edges in the HAZ of the cut. Second, I would check with the material supplier. There is a lot of garbage steel on the market that really doesn't conform to specs. We've had parts that have been fine for years, and all of a sudden we'll have a batch that is extremely hard, to the point of brittleness. I suspect this is the case. Ask your supplier for certs, and if he doesn't have any, its gray market steel that has been imported as one grade and being sold as another. A good share of the discount service centers handle this stuff.

 

[CoryPad]

I assume you are using cutting taps.

My USCTI chart shows the following for a 10-32 threaded hole:
[tt]
Tap drill size Theo. % thread
-------------- ------------
5/32 83
#22 81
#21 76
[/tt]

For an M6 threaded hole:
[tt]
Tap drill size Theo. % thread
--------------- ------------
#10 84
#9 79
5 mm 77[/tt]

 

[shorton2]

It's definately waterjet cut. They have a laser machine, but I now the look of the cut. As for steel, it is possible it's not to spec. I don't have the tool to check it's hardness. But, FWIW, I bought some taps that were supposed to be for pretty hard steel just in case that was an issue. Broke both today

Coreypad: Thanks.

* Is the USCTI chart on line somewhere?

I've got the Machinists Handbook, in case it's in there. But I didn't see it.

Looks like your smallest drill is bigger than what I'm using in both cases. I've been using a #11 for the M6. Perhaps that's part of my problem, particularly if the steel is harder that will aggravate the problem. I'll order some of those drill bits with my new tap order.

* any suggestion on taps or coatings for this potentally harder thatn spec steel?

* What about cutting speed? What rpm should I cut these at?

Thanks guys for the help.

 

[CoryPad]

The USCTI information is no longer available for free.

I have the 20th edition of Machinery's Handbook. It has recommended tap drill hole sizes in Table 2 of Section 10 Threads and Threading.

I recommend you work with high-end tap manufacturers like Emuge, OSG, and Sandvik for a specific tap and coating.

 

[shorton2]

Thanks, I'll check them out.

 

[CoryPad]

FYI, the Mach. Hand. info is the exact same as my USCTI info:

10-32 uses a 5/32 drill, while an M6 uses a 5 mm hole.

 

[shorton2]

Well, I have the 27th edition. I trudged through it (again) looking for the info. 2000 pages of threads, I found a table 2 which list sizes. But no where do I see anything that reflects drill sizes and expected overages or percent threads. Except a formula. I can run the formula, but I think I'll just try your drill sizes above if I can't find anything else to lookup...

 

[hydtools]

Here is Kennametal data that may be helpful:

http://www.widia.com/images/pdf/tec...f;jsessionid=LR5ZBHETMFEPLLAUBIOCFEVMCQFB0IV0

Ted

 

[mrainey]

And don't forget to check your tapping head for possible problems.


Software For Metalworking

http://closetolerancesoftware.com

 

[BobM3]

Have you tried thread forming taps? I have more luck (less breakage) with them. Do you need the full strength for the thread? If not then drill it a bit bigger.

 

[shorton2]

Bob:

I have not tried thread forming. Figured that would be harder with a manual maill and limited lubrication abilities. I do need full strength and an excellent fit for the application.

 

[shorton2]

>>Here is Kennametal data that may be helpful:

Ted, thanks, that was very helpful. Drill sizes with expected %thread results, and a nice recommended rpm table by material and hole sizes.

It looks to my one of my root problems may be determining what size hole my drills are actually producing. I'm using modern, high quality coated screw machine drills in a presicion chuck, so maybe I'm getting better results than the theoretical .003 oversize.

But I don't know how to measure the holes accurately. Can someone advise the correct (and most affordable) way to check hole diameters for this application?

Thanks guys for all the help.

Scott

 

[hydtools]

Make gages to inspect for minimum and maximum hole.

Ted

 

[saberblue]

A very heavy duty specialized taping compound might help as well here is a link to one of many

http://masterchemical.com/db-docs/pdf_di/TAP_LIGHT.pdf

A.R. "Andy" Nelson
Engineering Consultant
anelson@arnengineering.com

 

[ornerynorsk]

A heavy sulphurized natural cutting oil might help. There are some very good synthetics, as well.

 

[shorton2]

I ordered new OSG taps today. Also ordered new drills in the range recommended. Ordered some plug gages to check actual drilled hole sizes. I was using RapidTap tapping fluid in the beginning, and more recently a non-sulpher based cutting and tapping fluid. I don't know if the problems started with the fluid change, dont' think so. But I will go back to the original or try something new.

Thanks for the suggestions.

 

[schwisd]

30 to 50sfm for mild steels.Take 60 and divide it by the major diameter. This will give you a safe speed, you can crank it up as needed. Have you trammed the head to the work holder? Rigid tap holders with morse taper have less slop then the tapmatic heads.

 

[shorton2]

Thanks. The Kenmetal brochure had everything I needed. I used the speeds suggested there, bought new OSG taps, bought the plug gauges and a variety of drills close to the size recommended. I checked the holes with the plug gages and found that indeed, my drills are doing better than the "probable" hole size in the charts. And I changed back to Rapidtap. With that I was able to make a successful run with no tap breakage and a good feeling thread.

Thanks guys.
Scott