[brian257]

I need to make some 6061 aluminum parts that have eight 6-32 blind tapped holes in each part. The parts are 1" thick and I need to tap the holes about 5/16" deep. I have 200 parts to do so I will need about 1,600 tapped holes. They will be done on my Bridgeport CNC conversion with Mach 3 control. I don't have an auto tool changer so using the minimum amount of tool changes or doing one operation at a time and constantly changing parts will be required. The parts will also take a fair bit of time to machine and not breaking off taps in them and ruining the parts is pretty important.

My initial choice was going to be a Tormach ridgid tapping head, but since I don't have good control of the spindle speed and it takes an undetermined time to reverse the head I don't think it will work well.

My second choice would be to buy something like a Tapmatic reversing head. With this it might be best to do the tapping on the Bridgeport under CNC control, but it also might be easier if I just drill the holes on the CNC then manually tap the holes on my drill press with the Tapmatic head.

My third choice would be to use a multi-flute thread mill, but I have never done any thread milling before and I am not so sure how well this will work with a small 6-32 thread and a ton of holes. Looks like the thread mills are upwards of $100 each and they will be pretty fragile at this small size.

So any advice on how would be the best way to tackle this?

[metalworkz]

If you decide to go with manual tapping I would recommend using a Procunier tapping head over the Tapmatic and check out the Balax roll taps which do not produce chips and the thread is roll formed into the hole. The holes need to be sized for the Balax roll taps and I believe the 6-32 is .125" diameter for roll tap. You should be able to set the depth and without chip accumulation the process becomes much more reliable and faster. You can even program the operation and get very good threads although you will need to apply some tapping fluid. I have many years of experience with CNC tapping machines and multi-head tapping set ups and the process greatly improved with 2B thread quality when roll taps were used. Hope this helps some.

[brian257]

Thanks Wes. I ordered a Procuiner head today and some Cleveland thread forming taps since that is what Enco stocks. I sent an email to Balax asking about which tap would be best and expected tap life for 3/8" deep holes, but no answer yet. I will play with the Cleveland taps when they come, but would you expect much better performance from Balax? Any guess on how many holes a tap should be good for?

[rcs60]

forming taps are the best for blind holes there are plug,bottoming and modified bottom taps depending on how close to the bottom of the hole you are going. Cleveland taps should be ok for 6061 we have been using balax 10-24 form taps for a part and have gotten over 20000 holes per tap i would expect the same for the 6-32 tap

[109jb]

Secondary operation using a pneumatic tapping arm with a thread forming tap.

[metalworkz]

I don't have any experience with the Cleveland taps, but with Balax you can expect as much or more than rcs60 has stated as long as the aluminum is clean(no abrasive dust in the holes. You can also insure the long life of the taps by using a good tapping fluid with them. Aluminum is very tenacious and requires the taps be lubed regularly, but with the roll tap there are no chips to deal with so cleaning the tap of chips and clearing chips from the work is not necessary. If the holes can be drilled slightly deeper to relieve for the end of the tap the bottom tap may not be needed, but often that is not possible.

[brian257]

Thanks again. I have an inch of stock to work with and only need the threads 3/8" so I am thinking that just drilling maybe 5/8 and not using a bottoming tap will work best. I like the idea of using the bigger drill bit than I would be using for a standard tap and not having chips. 20,000 tapped holes per tap is 10 times what I expected so if this goes as planned this seemingly hard job just got very easy.

[rcs60]

a formula to use for drill size for a formed tapped hole is( major dia.-.0068*%thread/tpi) a 6-32 would be .138-.0068*60/32=.1252 drill for 60% thread for 85% thread it would be .120 drill #31
the machinist handbook also has the drill sizes in it for form taps i believe they are termed cold forming taps in the book

[brian257]

I got my Procunier tapping head last week and tried some tapping with the Cleveland forming taps in 1/4" aluminum and also a bottoming test at about 3/4" depth and it looks like this setup is going to work fine for what I need. Thanks again to those that helped. Looking at the taped holes they don't look great with a magnifier, but they seem to hold the screw just fine. I have some Balax taps and the correct size drill bits on the way so I expect them to improve.

One more question I have is when tapping to 3/4" depth with a 6-32 forming tap should I go part way and back off like I do with a cutting tap or just blast the full depth before reversing? Since the main reason for backing out with a cutting tap is to clear the chips I don't know if it is still necessary with the forming tap.

[metalworkz]

Keep the taps well lubed and you should not have to retract until the depth has been reached. Use a good tapping fluid and keep the taps lubed and I do not think you will have any problems. The threads the roll tap produce were much more consistent and it is a lot more easy to maintain 2B threads with the roll taps than with cutting taps and a lot has to do with chip build up both in the part and on the tap itself.