Tap Life

[Rakesh]

Hi guys,

I know there are very good machinist on this forum and if any body can help me.

I am machining a housing and the material is AL 6061. This housing have 175, M3 tap holes and is 8 mm deep. Right now, I am getting 1750 threaded hole per tap and tap is breaking. I am using Matsura RA 2G, matsura 660 and matsura 1000

Using osg drill 7/64, .450 deep hole with stub drill(I cannot go deep with depth Limitation). Rpm 4000 and 40ipm and giving 2 pecks. External coolant. After dill chamfer with carbide drill mill,giving 90 deg chmf. Than using 7/64 end mill plunging in the holes with G81,s6000,F60.

Than using Ballax Roll tap M3 going .35 deep and use S2000 with rigid tapping. Before Tapping is moo,The operator have to blow the holes and put oil in the holes and cycle start. We don't allow operator to stand there and again put the oil on the tap. I am getting 10 pcs per bright tap.

Now I am thinking to buy some high performance tap or use different approch to get more life out of tap. I am also thinking to buy carbide drill to get the straight hole from the drill. Other thing I don,t want to use oversize drill because Minor dia. of the thread is very important.Please help me I have to make 2000 more these parts.

Thanks in advance

[Guest]

I'd suggest buying some more taps.

 

You're going to need them.

 

Those are pretty good numbers, I think.

[Bruce Caulley]

You have 1000 to do, but the operators are manually putting oil on the holes?

 

Definately try a coated tap and increase coolant concentration , but 1750 holes per tap isn't too bad.

 

Bruce

[c-hook]

You shouldn't have to have someone standing there applying oil to a tap for that many holes (especially for aluminum), a properly concentrated coolant should suffice just fine. But if you are getting that many holes out of one tap, that sounds pretty optimal to me. There is a fine line between optimal tool life vs. optiomal speed. If you are looking to get longer tool life, you might want to try slowing things down a tad. I know this might sound crazy, but in the long run, it could save you time and money because you won't have stop production to replace taps.............My 2 cents.

[Guest CNC Apps Guy 1]

I'm with the majority here, that is pretty good life . You may want to look for taps with coolant through ducts and get a high pressure colant system. This is probably going to give you the best life/speed possible IMHO. Also run the coolant concentration higher as was stated earlier.

[machtek]

I'm also with the maj. on tap life. Do not use coated taps with alum, they will foul. I also think oil is a problem, use soluble oil instead of synthetic coolant, also do you have to use a rollform tap, SP FL cut tap for blind works ok for me. Thats my 2-cents

[Bruce Caulley]

quote:

---

Do not use coated taps with alum, they will foul.

---

If you use the wrong coating a rolltap will foul no matter what the material. TiN is appears to be the worst culprit in ally, but TiCN seems to go OK.

 

Bruce

[35K chipper]

M3x.5 rolltap should be drilled with 2.5mm > 2.6mm drill. use a carbide circuit board drl. cham hole 120 deg 3.15mm. check feed per rev. use all the control will allow. fpr.5mm = fpr .019685039in. if your in inch mode your tap makes 16 turns to the depth. if your feed per rev is off by +-.0001in. the deeper you go this small amount adds up quick. make sure you use a rolltap with a hydrolic releaf. richen your coolant, blow holes clean. hope this some help.

35k chipper

ps. i think matsura's will take 5 or 6 dec. places in rigid.

[Rakesh]

2.5 mm drill is for cutting tap. I am using the Roll tap. Second the circuit board drill also known as mini drill and use many time but at differnet situation and get from Metal Removal.

Circuit board drill have a very week web. I never have a problem using the osg stub drill and some time drill from Nachi and give a pretty straight holes. For improving more I ordered drill which is solid carbide which will drill .450 deep and also will give chmf on the top. I guess on monday I will leave the moo, to blow the holes and take off the oil and will provide the coolant.

I use Trim E206 coolant.

Anybody heard the carbide tap. I never use it. Any idea how it will perform in this situation

thanks

[35K chipper]

I stand corrected should be a 2.8mm drl. I've used carbide cut taps in 440c stainless at 35RC. if you can find a carbide 3x.5 roll tap it will last longer.

[savagkd]

Look into Emuge "Thriller" thread mills Linky they drill, chamfer, and thread mill all in one shot. Spendy, but you can get 5000 holes in aluminum at just a few seconds per hole

[toolall1]

quote:

--------------------------------------------------------------------------------

Do not use coated taps with alum, they will foul.

--------------------------------------------------------------------------------1750 holes per tap isn't too bad.

[5 AX]

I use BALAX 1.0 and 1.2 taps every day in 6061. I average over 2000 holes per tap. If I had to stop and put oil on the tap before tapping I would be out of business. My taps are chrome plated by BALAX, this helped a lot. My coolant is semi-synthetic. You should not have any problems increasing your tool life by going to chrome plate.

[Rakesh]

My three machines are running with high performance Nachi m3 roll with DLC coating. I already did 6300 tap holes per machine and same tap is still running in all the three machines.

I am getting high performance tap from Ballax than I will see how that will work and keep you guys posted about their performance.

Thanks for everybody for sharing their experiences and hope this thread will still cont.

thanks

[machtek]

Glad to hear you found a combo that works. Are you still using the oil or just the E206 (we like this stuff). What is DLC coating and what color is it?

 

Thanks