Tapping

[BrianP.]

Lately we been snapping more than a few taps. Wondering what people use for taps? Feeds and speeds? Coolant or tapping fluid? Roll or cut? Mostly in Aluminum but we also do steels and stainless.Doing some large Aluminum plates. M3,M3.5, M4, M6, and M8 holes. Larger taps no problem. Started with problems on the M4 holes. Got that straightened out and now M3 taps are going like crazy. Tried roll and cut. Gun and high spiral. Also drilled hole to high side at .1015 instead of .0984. Starting to really tick me off. Oh yeah rigid tapping in Haas VF-6 ( always seem to get stuck on the large machine ). Set for double retract speed then went to normal retract and broke another tap on 3rd plate. :wallbash: Other people are having some problems. Trying to get the owner to but a tapping arm to tap out side the machine. There are over a 120 different tapped holes in each plate. Starting them in the machine and finishing by hand could take a while.

[PLANET]

How deep are the holes?

 

Have you tried peck-tapping?

 

Also check your coolant mixture.

[Bruce Caulley]

A good roll tap and the coolant percentage set at max should be fine. It may be the machine though. I had a 50 taper machine once that the smaller taps needed a floating chuck even though a rigid cycle was being used.

 

HTH

 

Bruce

[Newbeeee™]

You could have a sync problem between the spndle and Z. Servos drift over time.

Hole size good?

Coolant strength good (and clean coolant)? We use 10% on everything as we cut everything.

Spiral flute BRIGHT finish. I really wouldn't use tin or anything coating that the reps tell you. I have never had luck with any and it wasn't through trying.

1000 RPM.

Tool in a hydraulic chuck (or excellent quality with zero runout).

R plane (start of tapping) at least 5mm from the job to let the axis/spindle sync

All else fails get a robodrill and do it at 5000 rpm

[jeff]

for aluminum I always use a form tap if I can. (we use OSG form taps)

we have a tapping arm , and i've found no better lube than WD-40 for tapping Alum.

 

also maybe try opening up the minor drill size a little bit to see if that helps.

 

Edit: just noticed that you tried the larger hole size...

 

 

When does it break the tap? when it starts to retract? Out of habit, I always have a small dwell 0.6 seconds at the bottom of the hole before it retracts, this seems to help or at least it has a placebo effect lol

[yorx57]

I use OSG hy-pro or the exo series taps and use a spiral point for through holes in aluminum. I used to have hit and miss issues

with my HAAS VF-4 until I came across a section in the manual and realized that there is a max spindle AND a max feedrate when

using the rigid tapping (I was always way over the max spindle). Now that I don't go over these maximums I have had no problems at

all with the tapping - actually doing #4-40 holes right now in aluminum.

[chris m]

Like the man said, keep the SFM down because high rpm leads to synchronization issues. We run a 7/64 drill for M3 roll tapping in 6061 and 7075 aluminum all day long with no problems; pushing the high limit on minor diameter, but in is in. 15 SFM with sh!tty coolant all day long with OSG Hy-Pro TiN 1.5P taps. If you want to spend a few bucks, call the Tapmatic guy and have him talk to you about Synchroflex. Tapping arms on the bench are a work-around, not a solution.

 

C

[jeff]

Tapping arms on the bench are a work-around, not a solution.

 

I would say it depends on the application, my guy pulls the part out of the mill, runs another one, and while that's running he taps the part.

Finished parts done quicker.

[chris m]

You have a point; my guys run [2] or [3] machines at a time, so not an option (or desireable for us).

 

What was that little guys name at the K who did the tapping, Brian; Hung, or something like that? Dude was a tapping fool.

[Joe788]

Lately we been snapping more than a few taps. Wondering what people use for taps? Feeds and speeds? Coolant or tapping fluid? Roll or cut? Mostly in Aluminum but we also do steels and stainless.Doing some large Aluminum plates. M3,M3.5, M4, M6, and M8 holes. Larger taps no problem. Started with problems on the M4 holes. Got that straightened out and now M3 taps are going like crazy. Tried roll and cut. Gun and high spiral. Also drilled hole to high side at .1015 instead of .0984. Starting to really tick me off. Oh yeah rigid tapping in Haas VF-6 ( always seem to get stuck on the large machine ). Set for double retract speed then went to normal retract and broke another tap on 3rd plate. :wallbash: Other people are having some problems. Trying to get the owner to but a tapping arm to tap out side the machine. There are over a 120 different tapped holes in each plate. Starting them in the machine and finishing by hand could take a while.

 

The only time we've ever had problems tapping aluminum, is when we tried switching to Oemeta coolant. We form tap from 0-80 to 5/16-24 at 2000rpm, millions of holes without a problem using Hangsterfers S500 coolant. For bigger than that, we go with spiral flute cut taps at their recommended SFM, with no problems at all.

 

My first guess would be your coolant. Second guess would be the machine. Third guess would be both one and two. What kind of coolant are you using? Do you have some floating tap holders you can try?

[BrianP.]

Thanks guys.The coolant is pretty new. I am going to juice it up a little more. Not sure which coolant we are using. I am not having problems with any of the larger taps. Going to go with the bright finish taps in the aluminum. Will check out the max spindle and feed rates for machine. Raise up the R plane sounds good too. May go to light oil when tapping. Just hate to stand there with a brush and oil for all those holes. All good suggestions. Really appreciate the suggestions. Can't get online at work so I do this on my own time that's why a slow response.

 

As for the tapping arm we have a couple of guys who do a lot of hand tapping so it would be of tremendous benefit to them. A huge time saver. The plates I am doing are 29.25 x 32.61 with a whole bunch of milling and other holes so it could be tapped offline no problem. Don't think I can fit them in a Rbodrill. At 15 SFM I think you could maybe tap faster with the arm. Good memory Chris it was Hung. We never tapped on the machines there and never had broken tap issues that I remember.

 

Well on to my next tapping adventure. 30 x 30 plate and 864 1/4-20 holes.

[chris m]

We never tapped on the machines there and never had broken tap issues that I remember

 

No, just parts with no threads in them from time to time, but considering how many holes that little dude tapped I don't think we had many problems.

 

I think that you could easily run 30SFM with Hy-Pros in aluminum, but you have to watch the RPM and feedrates so you stay in the machine's happy place.

 

Good luck

[BrianP.]

Well doing 864 1/4-20 holes. Made a fixture plate with clearance holes under the 1/4-20 holes so I could use a gun tap and bolt part down with existing holes. 15 SFM=229 RPM's. So i went with 200 and feed of ten. No broken taps but about 2 hours of tapping. Only 6 parts on a job that will probably not repeat so I can live with it. But it is painful to watch a machine go that slow.

[yorx57]

Well doing 864 1/4-20 holes. Made a fixture plate with clearance holes under the 1/4-20 holes so I could use a gun tap and bolt part down with existing holes. 15 SFM=229 RPM's. So i went with 200 and feed of ten. No broken taps but about 2 hours of tapping. Only 6 parts on a job that will probably not repeat so I can live with it. But it is painful to watch a machine go that slow.

 

That's the max spindle speed (200) on my HAAS VF4 for rigid tapping, but like I have posted earlier I have had no problems as long as I stick to that. It may be painful to watch, BUT it has been 100% reliable for me

 

Just as a side note, if you haven't done so already, check your owner's manual, there will probably also be a max feed - my specs (according to the manual) are max spindle 200 or max feed 100 - I can not exceed either value.

[McLaren]

Threadmill?

[JAMMAN]

I use the OSG Hy-pro taps also, for 1/4-20 through 3/8-16.

 

I can get 100's of 4-40 holes in CRS on our haas minimill with a simple 2fl gun tap. Nothing special on coolant but on tapping I always go slow... about 400 RPM for the 4-40 and about 250-350 with everything else. Those hy-pro modified bottoming taps are awesome and you have to love what they do with the chip. All rigid tapping.

 

Our Fadal I still use a rigid holder or collet even though it don't have real rigid tapping. Just go slow, works for me.

 

I do a lot of thread milling, almost daily. Bought a little 3/8 dia 6 fl solid carbide with a 3/8 shank and a 1/4" dia relief, TiAln from Harvey tool. I finished 32 M12 X 1.5 holes today, no notable wear. Use it as a single point. I did the outside threads on these parts on the mill also because the lathe was tied up. Best 60 bucks I ever spent.

[gms1]

I use the osg hy-pro with black oxide finish on all our aluminum parts too. I never roll form in aluminum cause I hate the welt it leaves behind at the top of the hole. The guys running the machines always break the thread when they try and chamfer the holes by hand. If I had my choice I would thread mill everything but that's inefficient apparently.