3/4-10 Threads

[patboyd69]

I have a job coming up that has 3/4-10  2B tapped holes 2" deep, ( 64 parts) and was wondering if anyone out there has done this on a mill?  Its a Haas VF-6, any tap recommendations would be helpful, or threadmill advice.    Its mild steel. Thanks in advance!!

[jlw™]

Do it all the time. OSG taps, leave room at the bottom of the hole for chips and tap to depth.

[patboyd69]

Its a thru hole, so that should be a plus.  what would you recommend for speeds?

[Guest]

Threadmill...done

 

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=993980

[Machineguy]

OSG has the high Helix taps for steel. They work well.

2" is deep for a tap, even with a reduced shank. I would say your borderline on going to a thread mill.

You got a holder that size? That's a #2 holder I think.

2B is hard to find in that size, that's why I say thread mill.

 

Also coolant need to be at 9% or so. Or use a tapping oil.

 

 

Machineguy

[patboyd69]

I would have to buy a holder that size also.  So, thread mill would probably be a better option...Plus I hate breaking taps!!

 

Thanks for the advice.

[AMCNitro]

Id go threadmill all day long on that.  Once you set your tool comp it'll run all day.  And think about this if you break a tap you chuck the part, if you break a threadmill part will probably still be good.

[crazy^millman]

look at advent. you could relive the shank and get the 2.00 length you need.

 

http://www.advent-threadmill.com/adventthreadmill/341058-bh3kl17

 

Draw a helix to use and then the arc3D chook to get good output.

[jlw™]

personally I'd tap that hole all day, especially a thru hole. It'll be faster. ours go 2.25in deep in A36 at 24sf with plain old machine coolant. That's with 3in stick out on the tap. We usually change the tap every 120 holes... It could go much much farther but as pointed out a broke tap sucks.

 

Having said that, in anything like p20, finkl fx1 or 4140 I always threadmill.

[jeff]

I'd use this tap:

http://www.mscdirect.com/product/details/58542028?rItem=58542028

 

a thru hole in mild steel definitely calls for a tap, you'll save a TON of cycle time.

[absolute technologies]

If you choose tapping, which IMHO is faster and has less tooling costs per hole when compared to thread-milling, you DO NOT want to use a spiral flute tap, they're only good up 2X diameter or less otherwise the flutes will pack up with chips and it will break. Rather you want to us a spiral point tap that pushes the chip in front, thru the hole. A spiral flute tap is the weakest type and a spiral point is the strongest other that form taps. Being the part is steel you would want either the Steam Oxide coating (black) or the TiCn coating and Powered Metal as opposed to HSS, like the OSG VC10 grade.

 

Cheers!

Len Dye

[Mike@Lustre]

Have to agree with tapping , buy a longer shank spiral point tap and let it eat , I prefer 3 flutes designs much stronger cutting profile

[patboyd69]

Thanks for all the great suggestions.