O/T tapping deep holes

[Shady]

Im hoping someone can give me some advice. I need to tap a bunch of holes 7/8 nc9 to give full thread all the way thru a 4" thick mild steel burnout on a vertical mill. Should I try an extended length tap or a threadmill? Im not experienced with either. I dont think an extended length tap will hold up. I have never used a thread mill, I have only thread milled with a single point internal lathe threading bar. Any help would be greatly appreciated....I hate taking these 300 lb parts off the mill to tap them on the drillpress to finish them. Thanks~~~~~~~Shady

[kccadcam]

I would go with Emuge extended taps:

http://www.emugecorp.com/

[crazy^millman]

Extened tap all the way if you got the machine and the holder to push it. I would not even think about thread milling this. I would think you are at the limits of most VMC's at the 7/8-9. I have done it but scared the crap out of me. I would get squre holder collet sysytem to hold the taps not a standard ETM collet. Problay peck tap it also like .1 to .2 may take longer but will insure you get the cutting fluid to the tap as well as the chip evucation you need for a hole that deep. If you got a radial drill press I reccomend using that frist with a square morse tap holder to drive that bad boy.

 

Crazy Millman

[PE @ IHS]

Give rollform taps a try. They seem to break far less frequently than regular machine taps. make sure to get the correct tap drill size (it is different from regular tap drill sizes)

 

Threadmilling works well, but tapping is much faster.

[Müřlıń®]

quote:

---

make sure to get the correct tap drill size

---

+1....I would cheat and go with a slightly larger drill size if I could and flood it with oil.

 

Unless they specify thread spec.

 

.01 bigger drill size will make alot of diffrence cause like Mill says, 7/8 tap takes a hell of alot of torque. I tapped enough of them by hand with a pipe with a socket welded in the middle of it.

 

Murlin

[kccadcam]

quote:

---

+1....I would cheat and go with a slightly larger drill size if I could and flood it with oil.

---

+2 on that, I've rigid tapped 1-8 threads with Emuge on a big Toshiba Horizontal, but we're talking serious grunt. What brand of machining center are you attempting this on?

 

I would peck tap at .5 and flood the hell out of it.

 

High pressure coolant thru taps would be the most ideal situation, G84 right on thru!

[Shady]

Thanks for the input. we are using a 2003 model Daewoo DMV 4020 50 taper. Peck tapping? I have never tried peck tapping...except by hand of course! We have a radial drill...but it is in our other shop...about 1/8 mile down the road from our CNC shop. We do "cheat" a little on the drill size...we would never get them done otherwise. I appreciate all the advice...if you have any other thoughts, please send them my way. I will let ya know what...if anything...works. Thanks everyone, ~~~~Shady

[Gary]

I used to do a bunch of these up to 1.5-12 on a 5 horse vertical mill. (Probally toughest was 1-8) Biggest thing for us was chip clearance under part. Pecking as stated above is also important I don't think it could be done without.

[dan m]

I dont want to sound stupid but i never heard of peck tapping on a cnc. You dont actually retract the tap all the way out of the hole do you? And if you do isnt there a chance of (for a lack of better words) cross threading the part?

[crazy^millman]

Nope a good machine tool is the key as well as a good holding system for the Tap. I have peck tapped 440 stainless 40 Rc and not have a problem with it.

 

The code for doing this is intrgrated in the control of A mazatrol machine which is a Mazak. I have also seen mention of it for a Fadal. The idea behind it is that you get the same effect as the hand method wit hthe breaking of the chips and allowing of the cutting and cooling action of the fuild to get to the point of attack so to speak. If you have a machien tool wit hrigid tapping and it orients to the same place every time which most do then you can write the tapping cycle as a depth change in .1 to .5 depth changes the key will be to keep the z height the same for the start as well as the feed rate and I would do the same depth down and do it as a even amount not an odd ball amount. Here is soem coe to give you an example of what I mean:

Z.1

G99 G84 Z-.2 R.111

Z-.4 R.111

Z-.6 R.111

Z-.8 R.111

ETC......

 

I know it seem simplictic but if you are worried paint a line on the holder and a one of the flutes to relation of the part you are tapping and just do a verification of proper starting. If you like this and want ot get really fancy you can use the Msic paramters on the second page as a control for a cycle of this nature.

 

Crazy Millman

[dan m]

Thanks Millman

After reading your reply it does make sence that should work. learned somthing new once again lol

[robk]

I will be the one to suggest thread milling. 7/8-9 is one of the sizes we machine on a regular basis in 420ss. We don't go that deep (only 2.875 as compared to your 4.00). The tool is a solid carbide single profile thread mill from MSC (part #40232993). You would have to grind down the shank dia. to get the length you need but that's about it.

[Shady]

Thanks again everyone....once again Im convinced...you guys know your...uh...shazbat. I really appreciate the help. I am really new to CNC work...only been at it about a year now...with no formal training so I count on this forum alot, and have never been disappointed. Hope I can be as helpful to someone someday. ~~~~~~Shady