Roll taps vs cut taps
What is the difference? I understand that a roll tap provides stronger threads correct?
Do I program them differently? G84 canned cycles.
Feeling a cut tap and roll tap in my hands how can I tell them apart?
Thanks a lot.
How much research have you done?
From tap has no cutting flutes. It will not have any sharp edges.
The only difference is that drill size. You need to be mindful of the drill size. Sometimes you need a metric drill to get it right.
Thread strength is really just incidental. The real beauty is that they last forever, break less, and are not material specific.
Looking at a roll form tap and you not see deep gullet type flutes, tho you may see something that looks like a keyway, so air/coolant can escape the hole.
Roll tap is a forming tool, not a cutting tool, treat it accordingly.
While they are not material specific, they do not work on all materials. There is a requirement that the material has to flow. More ductile materials work better. A lot of plastics dont work so well....
Roll taps DEMAND a more consistently sized hole. This cannot be stressed enough.
Plus side for roll taps
They're really hard to break
Thread can be stronger.
The threads usually don't look as good as a cut tap
They tend to pull material up around the mouth of the hole. ( Need a bigger countersink)
They're best in ductile materials like aluminum.
Require more precise hole size.
Anything that make stringy chips can be form tapped.
Originally Posted by John Welden
They work great in AL, but are also great for steels under 35Rc, stainless, brass, copper, and some ductile and malleable irons.
Once you get up around 5/8, form taps are not as advantageous IMO.
I forgot a form tap pro.
It's easy to tap threads right to the bottom of a hole. They have minimal lead.
I love form taps for small blind holes because I don't have to worry about pulling out the chips. I always believed the stronger thread story, but then I read some tests where, in practical applications, there wasn't much difference. +1 about hole size. It needs to be exactly right to get all the benefits. Form taps seem expensive but in the long run they're way cheaper!
are they has good on a manual mill like they are on cnc mill i ask my boss to order some last week to try them out in SS304 but didnt had time to try them but on the first look they dont look any stronger than a spiral flute tap so how are they harder to break since you need more force to form a tap instead of cutting it ? if someone can clear this for me would be nice
If you drill the right size hole, a form tap in 304 will come out looking truly "groovy"! It's all about the fit and the lube.
The tap drill required for a form tap is larger than a cutting tap.
The tolerance on the drilled hole is much less than with a cutting tap.
The form tap has no sharp edges that can dull, and no chips to control.
I also use them to "repair" threads that have peen "pulled" so I can use a longer bolt, or cross threaded so bad a bolt can't be started straight.
For threaded thru holes I tap from the undamaged side.
For a blind hole I thread them in till it is touching the undistorted threads, back out slightly and hit the end of the tap lightly with a hammer, back out a little more and repeat several times till I get a turn or more on the orig. threads, then continue tapping to the bottom of existing threads. Then switch over to a cutting tap to cut the threads deeper.
"A lot of plastics dont work so well...." I was trying to tap 10-32 blind holes in Delrin, H13 taps still came out undersize for a Basic thread size.
Save the nice sharp cut taps for plastics only, they do not form tap well. Ductile metals will take form taps nicely and give you very good threads. Harder or more brittle metals do not form tap well and need to be cut tapped.
Originally Posted by hitandmiss
Important to note if you are trying to 'fix' the depth on a form tap..you cannot re-drill them deeper.....the tap drills sizes for them are larger than the minor diameter of the thread...the form tap forms INTO the hole...
Yes the only way to make a form tapped hole deeper is to drill for and use a cut tap.
After having problems in soft materials, aluminum, 12L14, etc , I quit using the form taps with the pressure escape groove down the side. That groove can become clogged with swarf in the soft materials causing way oversize threads and/or early tap breakage.
Originally Posted by Chobyn
Instead I switched to OSG brand taps with a four lobe, squarish cross section for pressure relief and no place for swarf to accumulate.
Form taps can far outlast cutting taps. Several did up to 4,000 10-32, 3/4" deep holes in 12L14. Trying to get as many holes as possible out of form taps, I learned a hard lesson about form tap's longevity. They wear on the ends from extended use causing the threads at the bottom of the holes to be tapered undersize so for long runs we made a practice to screw a thread gage to the very bottom of the holes.
Occasionally, I had the first few threads of form taps break off from extended use, hitting the bottom of a hole or such. In a pinch the taps can be salvaged by spinning them in your fingers against a grinding wheel to form a new taper on the end. Probably not a recommended procedure even though the resulting threads never seemed to show any difference.
And the form tapped hole needs to be tapped all the way to the bottom so that the chips from the cut tap don't expand into the larger form tap hole and pull out the threads on the way out. Not likely to happen with stainless but very likely with something softer like cast aluminum.
I have had the same problem as well. I was throwing it out there as that might be an identifying feature he might see.
You might find this helpful http://www.f-m-s.dk/1.08.pdf
Originally Posted by MBG
To me the biggest disadvantage with rolling external threads is that standard OD material for thread rolling isn't normally available.
For an external thread the OD must NEVER be larger than nominal pitch diameter and for internal NEVER smaller than nominal pitch diameter.
You can even roll tap materials like 4360
I had 36 M8 * 18mm deep holes to tap per cycle, and using a spiral form cutting tap resulted in lots of stringy chips everywhere, even with a chip breaker tapping cycle.
Emuge PM roll tap would last 25 cycles on average (it was changed then because we did'nt like losing parts to a broken tap) and thats with regular oil/water coolant.
Only drawback was making sure the counter sink was deep enough on top of the 7.4 hole wacked in with a stellram hardcore drill (24"/min feed mmmmm )
Form taps don't really have flutes to weaken them. Spiral flute taps are among the weakest taps out there. The form tap is basically a bolt made out of tool steel, so its body strength is very high. But its not ductile, so they can get stuck and break if shock loaded.
Originally Posted by Krovvax
I'm not sure how good a start you'd get using form taps on a manual mill, because the tendency to "lean on 'em" to make them start is quite high, and this could damage the first few threads, unfortunately, those ones count the most.
I have been using form taps for almost a year now. 5/8 and 3/4 diameter. In 4140 and 4340. Didn't really like them at first but now prefer them. They do last a lot longer. Just wondering if you guys think rigid tapping is better than a floating tap holder for form taps. Seems obvious to go with rigid b/c of pressure needed to get started, but asking anyway.