I had never really messed with form tapping, now I'm running two jobs with it at the same time. Both are in 1018, tank stuff. One is 3/8-16 half inch deep, I've run in between 40-80 sfm and an 11/32 drill. The threads are on size, but they look like crap, I went back to a cut tap on this one.
The other is 1/4-28 full form to 1" in a blind hole. Running an A drill, the treads look pretty good, when they stay with the part. Wrote the program yesterday, and had another guy (we'll call him Jose) set it up. Came in in the morning 2:59am (couldn't sleep) and the program has run, the first parts are in the vises, ops 1 and 2. Cool. Threads look good, the second op looks good, except, threads are undersized. Run a piece of scrap, threads are undersized. Running 250 rpm 8.964 or something IPM. Hmm slow it down to 5ipm, with coresponding RPM change. Oversized threads, Interesting, so I spent 3 hours messing with speeds to try and get a good thread on the Go/NoGo. Turns out 7.5 ipm gives an oversized thread, 8ipm gives an undersized thread, and 7.75ipm gives an oversized thread for the first half of the hole, and undersized for the bottom half, screw it, theres only 50 parts with 1 hole a piece, I'll just have a part timer chase them. (I'm not being mean, they get to sit in a recliner in front of the swamp cooler while they are doing it). Now the problem is chasing with a form tap, they threads are either good or big, crap, try a cut tap, and ripped all the threads out.
My 'lubrication' method from my 3 hour experiment this morning was that flood coolant was out, tap oil was OK, but still losing some threads (tapmatic, not tapmagic, that smells good). I was putting some tap oil in the hole, making sure that the tap was clean (visual and air blast) coating that and then putting some synthetic grease on the tap and in the hole, then adjusting that to following the tap with a brush and making sure on the pull out that the tap was covered in oil. That prevented the top few threads from ripping out.
So what am I doing wrong? I'm thinking that these 1/4-28 taps blow. We ran a bunch of nuts on the lathe in 416 with 10-32 threads, and they worked just fine, though the tap was basically round, these have a slight square shape to them.
Are you using a spring loaded tapping spindle
or are you riggid taping? Machining center or
manual mill? I tap 1018 5/16-18 1" deep on
Bridgeport manual mill all the time, just use
regular R-8 collet, I am pretty good on exactly
when to hit the reverse switch to back the tap
out, I use either 2-flute straight or 3 flute
spiral OSG taps, black oxide. I spray WD-40
with free hand, RPM range anywhere from 90-190 rpms depending on how many beers I have had.
I "never" have used a form tap, cut taps only.
Alignment is very important if tap goes in
just a few .001s off center it will tear the
hell out of 1018.
We used a lot of form taps when I worked in a screw machine shop. I do know that hole size is critical, not only to keep the tap from breaking, but to have it displace the material necessary for a good thread. If your threads are getting ripped out, it sounds like the hole is too small. Also, I would suggest using a spring-loaded tap driver.
I'd try a different size drill and or tap
Dualkit, I've done that many times also with a cut tap, but this is rigid tapping on CNC, though I always put the tap in a drill chuck(crappy one), instead of a collet so it would spin before breaking with clogged chips.
The 3/8-16 hole was on a Mazak FJV-20, I'm not too worried about this one, it seems to me that form tapping works better on small stuff. The 1/4-28 was on a Fadal.
The 3 hours this morning wasn't just messing with this, I was keeping the other mill running (end of the quarter and all). Most of my time was spent with feeds and speeds, 7.5ipm consistantly big, 8ipm consistantly small. I also spent a bit of time resetting the backlash in the Z, swapping out drill sizes and verifying the other two ops. Yes the 3 hours bothered me too. This is one of those jobs that has to go NOW, so waiting another day for more taps wasn't an option, I had to make due with what I had.
This is a Fadal, so I'm a bit skeptical of its capabilities. I tried 15ipm(420 rpms) and the spindle didn't stop in conjuction with the Z axis and pulled the part about .05 out of the vise, no broken tap though. I should be using a floating tapping head, though once again, higher speed smaller thread.
I did try a B and a C drill, didn't seem to make a difference, went back to an A, the minor diameter is good, a bit on the high side. The thread tearing wasn't due to a small hole, it happened on the reverse, that was a lubrication problem.
1" full thread on a 1/4-28 is fairly deep. The tap goes in, the treaded part goes in, the skinny neck goes in, and the collet nut almost hits the part, is this part of my problem, or crappy taps.
Is this a common problem, with over/undersize threads, what size drills would you guys run, speeds/feeds. Is this a problem with the Fadal? and its total inabilitly to change direction, or do these taps just plain old suck, thanx for the input
I use form taps a lot on my Fadal. I use rigid tapping, and put the taps in rigid holders. Fadal recommends not using spring loaded tension/compression holders for rigid tapping. The machine is quite capable of rigid tapping. I do it all the time, and sometimes at over 1000 rpms. You mentioned that you were putting taps in a drill chuck. This could be the problem. Is that tap slipping in the drill chuck occasionally? That would explain the inconsistency. Usually, if threads are size, they stay there untill the tap wears too much. Not size one time, then big the next. Rigid tapping is not just the job of the machine, it's also your job to make the tap rigid to the spindle either by a holder specificly for taps, or at least a collet.
you are tapping toooo slow.
yes use a spring loaded holder.
with a a spring holder feed in at 97% of the thread lead.
make sure ou have the proper drill. machinist handbook has roll tap drill sizes.
use a quality tap like emuge or osg
420 rpms at 15 IPM is right on the money as
far as matching the thread lead, but rigid
tapping only works well under perfect conditions.
If that machine is off a little on that 420 rpm
or 15 IPM it will be either shoving the tap
ahead of the thread or trying to pull the spindle
down with it. Get a spring loaded tap holder
and run it at 14 IPM at 420 and use that nice
forgiving spring. You are drill and tapping
in the same chucking/clamping right?
Well, I see I am out numbered about the rigid holder. I know it will work with the tension/compression holder, but don't expect real accurate depth control. On the fadal, if you program 420 rpm, you won't run exactly 420 when rigid tapping. The machine will adjust accordingly to match the feed. It will be sinchronized to the Z axis. The only way this will not work is if the rigid tapping is not working correctly. I've used rigid tapping with rigid holders for 6 years now with no problems. All 6 years were on my Fadal. I ain't arguing with anyone, but rigid tapping is called rigid tapping for a reason. The spring holders will work just fine, but you then might as well not use the rigid tapping code. This will save you some cycle time as the spindle doesn't need to orientate to find itself on the first hole.
Dave K, no hard feelings! I am just anti-rigid
tapping because of all the variables that can
kill it whether it be on a mill or lathe.
An old/sloppy encoder belt, bad holder , spindle
out of alignment etc,etc can cause problems
that a spring loaded one will forgive. I have
seen CNC Screw machines only a few months old
that could no longer rigid tap because a crash
misaligned the tapping tool to the spindle
by .003 and a spring loaded one didn't care.
Just trying to provide the method that will
work under the highest percentage of circumstances.
My question is, how can you get an undersize hole with a form tap?
I use express taps ( form Taps) all the time on my Fadal. Rigid tapping, No spring holder. Indicate your tap to make sure it is running true. Check hole size to make sure drill is cutting to size. Balax has Tap charts for express taps. Hole size is absolutley critical to end up with correct minor dia. I use a mix of lanolin and moly-dee when tapping steel. 1018 doesn't finish great no matter what. 1/4-28 I would start about 800 rpm. Resist the temptation to run too slow. Form taps create incredible amounts of tension on the tap. A little inertia seems to help. The critical thing I believe is lube. The moly-dee does real well in pressure type applications. I like Balax taps real well for roll tapping.
Good luck Bob.
Oh, I meant to add. Fadal sells a special tool like a big acme thread to do rigid tap testing. If your ramp and gain are off you will go through taps quicker than a nine year old with a box of chicklets.
Absolutely no hard feelings taken, and I see your point. I guess I'm just a little biased toward rigid, because I've seen it work so well for many years. I consider it proven technology. Your points are well taken.
Thanx for all your relies, and now that I'm not so tired, I might make a bit more sense. First I wasn't holding it in a drill chuck, that was a reply to someone talking about tapping on a manual machine. Doug, it wasn't an undersized hole it was an undersized pitch diameter, but only above 217 rpms, below this, oversized PD.
As far as tapping at over 1000 rpms on a fadal, I would be scared at 420, the spindle overran the Z on the reverse.
Anyways, I think my problem was crappy taps, ran them at 224 rpms, 8.ipm, a little under size and just chased them. No biggie, but still a pain.
Now on to the next adventure, whats the quickest way to tap brass? and the quickest way to hog 17-4?
Bob, you may have just clued me in on that statement. The only time I've seen the spindle overun the Z, is when you are using the conventional tapping code. Are you sure you are using the G84.1 for tapping and not the G84? You will get that overun on conventional tapping.
the spindle overran the Z on the reverse.
I use form taps all the time - but I seldom ever run 1018. Generally in alum or 1215 or 12L14. I generally run a smaller (sometimes a lot smaller) drill than recommended and bring my crests right to the top - and run that way all day.
I run them in oil or coolant. I always have them in a floating holder of some sort. I think that is where your size trouble is comming from. And possibly your ripping?
I generally run TiN coated taps. From your description I am wondering what surface treatment your had?
A form tap shouldn't run undersize untill the crest of the tap is worn down. And then only to the last thread or two. You must not be holding your mouth right.
I run rigid in one lathe. I have a 3/8-16 in the crossworking that lives forever that is rigid. But for the 3/4-10 endworking - I opted for a Tapmatic holder made for rigid applications that gives a tad movement in Z just to absorb any following errors - yet still gives reliable depth control, and it also allows for missalignment radially too. Even the 3/4-10 lives a good life. (1200 series steel) Both on this job are cut taps tho.
Think Snow Eh!
I am with Dave K. They call it rigid tapping for a reason. The thought about the tap slipping is something to think about. I've had it happen myself. I've made some adapters to hold taps with 2 opposing screws to lock on to flats ground on the tap shank, which I put into end mill holders. Never a slipped tap, and no more ER collets trashed from the result. Have you determined that your drilled holes are consistant for size and are straight? Blowing chips out of the holes? Moly-Dee? 1018 does suck, I am into some of that currently, as well.
That was the weird thing, holes were fine, chips blown out. Using tapping oil and a Mobil synthetic Milblahblahblah grease left over from an assembly. The ripping of the top threads was fixed by adding some more oil into the hole when the spindle reversed. The minor diameter was good, but I could not get a good pitch diameter, big pitch diameter at 7.5ipm and 210 rpms and lower, small pitch diameter at 224 rpms at 8ipm and greater. I changed taps a bunch of times, they were OSGs, one of the darker coatings. Both jobs are done and we might see them again or not.
I think I'll experiment a little more with form taps, I really like the speed you can get out of them, you guys have been helpful, but I still can't figure out why I couldn't get a good pitch diameter.
The opposing screw idea, is that in a hard holder? and does it screw up your run out?