O/T Checking Roll Form Threads

[GREG]

Hello All

We are starting to use roll form taps a lot more on materials other than aliuminium. (stainless, copper,steel,tool steel ect.)

No problems with the taps or tool life, in fact much better results than with cut taps but not achieving core diameter even though thread gauges

OK with NO/NoGo gauge.

QA are all over this and we are scrapping good parts in my opinion.

Can anyone point me to a procedure / tolerances to measure internal roll form threads or any other infomation that may help.

 

Cheers

[Rekd™]

Your drill dia will likely be the deciding factor in the minor dia's final outcome. (Note that it is not created until after the tap runs, forcing mat'l back into the hole.

 

I believe they must be guaged the same as cut threads.

 

'Rekd

[crazy^millman]

+1 Might need to look at reaming your holes verse just drilling. Been my experience that drills have a way of making holes different than you want. The reamer should also give you a better RMS in the holes which help the roll forming process. I would do a go / no-go on the holes about every 100 to 200 holes and get a 100% inspection there before forming the threads. It would also do you good to experiment on the different material and what hole sizes produce the best reults. Different Material do different things and Elogation and Tensile strength and other things come into play as well as the elastity of the material to give the results you are after. If doing class 3 threads the holes size difference of .0005 can make or break a part if roll forming anything smaller than #10. You may also find in you are not reaming the holes your inspectors could be failing the parts on true position. A .005 true postion only gives you a maxinum devation of .0014 in both axis direction. Big mistake most engineers make is that freaking true poistion. I have had .002 true position call outs of casting as well as .002 profile callouts on delrin. I can hold the material in my hand and change it more than the spec's on the print.

 

Good luck and just take more care on the apporach it pay in the long run to take an extra few mintues per part verse losing the whole thing.

 

HTH

[?Mark]

Another thing to tell your insp. people is that even though hole size will always be a little bigger that after cut thread, thread itself will always be much stronger when formed.

 

Mark

[GREG]

Oh to be able to tell the QA people something.

I dream of such a world.

Thanks for the replys.

We are using good quality drills capable of H7 tolerance holes that are checked regulary and for the most part we are producing good quality tapped holes that gauge fine.

Its the grey area between a perfect thread to the engineers book ( QA ) and what is actualy practicle in a production inviroment.

Any help is greatly appreciated.

Cheers

[gcode]

I believe that a drill size chart for cut threads

is calculated to give 65-70% thread.

Rolled threads will never achieve that. Most rolled threads come in at 50-55% thread. Despite that, a rolled thread is almost alway stronger than a cut thread.

The smaller the tap, the higher tolerance you must hold on the drilled hole to get a good pitch diameter.

I generally ream when roll tapping 1/4in and smaller.

Some customers will not buy rolled threads because the minor diameter does not meet cut thread specs.

Try contacting customer support for your roll tap

manufacturer. They may be able to provide you

with reports and studies you can use in your war with inspection.

If you can't win over your inspection department,

go straight to your customers. If you can convince

your customer that roll tapped threads are

stonger and more economical to produce, inspection

loses by default :-)

[chris m]

We form a lot of threads here and sometimes run into this question. I typically use a tap drill selector published by a tap manufacturer [OSG and Balax have pretty good charts] instead of the 'wall chart' because I have come across some sketchy wall charts running around

 

I typically pull out the Machinery's Handbook and try to convince the designers that as long as I'm under the 'Maximum Allowable Minor Diameter' in the chart we're OK.

 

C

[Rekd™]

If you guys are interested... you can have this..

 

 

I'll put up a link later.

 

[edit]

It's on the FTP, unspecified uploads. There's 2 files, download the one that says setup if you don't have the VB6 runtime files.

[/edit]

 

'Rekd

[F. JAVIER]

An important detail on smaller thread sizes is that the drill size sugested for roll is not always at the ideal chart size and if the hole starts bellmouthing the thread minor will not be forming fully in the area mentioned and for that reason you should take extra care in small deep roll formed threads. (or ream as suggested)

I would sugest to check from the end side on thru threads and if blind to do a test at the same depth (but thru) every 100 threads (or whatever you choose) to insure your quality.