[Shotout]

I have a job that woud require 40 3/8-16 x .5 in DOM tubing. This will be a recurring job, monthly, for several months. I was wondering if threading milling woud be the most effiecent process for this. Otherwise I'm stuck ridgid tapping and just don't feel like that would be the way to go. I was looking at something like this tool: www1.mscdirect.com/CGI/NNSRIT?PMPXNO=4412214&PMT4NO=32481809

I've never thread milled before, do have cam software to program it though, and would appreciate any help or suggestions.

Thanks
Scott

[Jcip]

Scott, Forgive me but what is DOM Tubing? Thread milling works great for certain applications, i.e. special thread size, tuff mat'l, accruate depth, But if you are just tapping 3/8-16 x 1/2 dp, rigid tapping is the way to go, it's much quicker, and the cost of a good tap vs. thread milling tool, well you can buy a lot of good taps for the price of thead mill tool. And with rigid tap your tool life should be excellent, Also your cam software may have threadmilling but does your /CNC have Helical cutting? You would be surprised how many don't.

Hope this helps
Jim C

[Shotout]

DOM= Drawn Over Mandrel tubing.
I have both the ridgid tapping and our mill will helical intrup so because of the depth and the interupted nature of the cut with the arc of the inside and outside wall I wasn't sure which method would be best. Our mills, Haas TM-1s have 7.5hp peak and I have had problems with smaller taps breaking in deep holes. I can peck in by 1/2 the dia of the tap, the machine will repeat on ridgid tapping, but that will take awhile. If I have to peck my way in I was thinking a threadmill program with a single point tool like the one I refrenced might be faster and because of the nature of the cut I was wondering if it would last longer. Would you still ridgid tap this? Thanks

Scott, Forgive me but what is DOM Tubing? Thread milling works great for certain applications, i.e. special thread size, tuff mat'l, accruate depth, But if you are just tapping 3/8-16 x 1/2 dp, rigid tapping is the way to go, it's much quicker, and the cost of a good tap vs. thread milling tool, well you can buy a lot of good taps for the price of thead mill tool. And with rigid tap your tool life should be excellent, Also your cam software may have threadmilling but does your /CNC have Helical cutting? You would be surprised how many don't.

Hope this helps
Jim C

[Geof]

3/8"-16 in DOM?

Much much quicker to tap. What is your wall thickness? You can probably do it with one pass; we do HRS steel regularly 5/16"-18 and 3/8"-16 up to 1/2" deep in a single pass on a MiniMill with the same power you have. Run at 1000rpm and use a richer than normal coolant mix. For a through hole use a spiral point tap.

[Shotout]

3/8"-16 in DOM?

Much much quicker to tap. What is your wall thickness? You can probably do it with one pass; we do HRS steel regularly 5/16"-18 and 3/8"-16 up to 1/2" deep in a single pass on a MiniMill with the same power you have. Run at 1000rpm and use a richer than normal coolant mix. For a through hole use a spiral point tap.

Wall thickness will be .500 +/- .001
At 1000rpm I'm getting a sfm of 93.75. I usually use about 80sfm for drilling 40% for tapping. Is that why I'm breaking so many taps? I run my coolant at about 20% when tapping, recommended is 8-10% for milling, counter sink holes to be tapped to the major Dia + 1/2 the tolerance to break edges and ease the entry of the tap and round my speeds so that my feedrate is no more than a 2plc decimal and use R.25 to make sure I have good coolant flow prior to the tap entering the hole. Normally the tap breaks at depth 2X the dia unless I incrementally tap to depth. Any thoughts or suggestions are appreciated.
Scott

[Geof]

Wall thickness will be .500 +/- .001
At 1000rpm I'm getting a sfm of 93.75. I usually use about 80sfm for drilling 40% for tapping. Is that why I'm breaking so many taps?.....
Scott

Do you mean you use 40% of 80sfm for tapping? In other words 32sfm which is 34% of 93.75sfm or 341rpm???

If you are running at this rpm that could be the reason for breaking taps.

I have found with tapping just about any material that sometimes the chips form nicer when the tap is running faster; they seem to peel off in nicer curls rather than folding up in the fluts and jamming.

Also on the MiniMill I have found that when the spindle is running down below 400 rpm it loses torque and seems to have difficulty maintaining synchronization. Down in the 200 region you can sometimes hear the spindle speed oscillating. I suspect breakage could occur at slow speeds because the synchronization is lost during reversal.

This was discussed, I think, in a recent thread; have you gone through any threads about tapping?

[Shotout]

Yes, can't remember where I read that as a rule of thumb to use about 40% but yes. Softer materials that chip well like aluminum (6061T 7075) and larger dia taps in mild I run faster as I noticed the machine ~seemed~ to want to stall the spindle just before breaking the tap so I assumed it was a torque issue and sped the speed/feed up to try and get more torque. But I also use the repeat feature of the controller a lot too to prevent tap breakage.

I have noticed the spindle speed will drop and the load will kick up to compensate but it is so fast, (our machines are older w/ CRT monitors) that the feedrate display doesn't change on the display so I've assumed sync was kept just not displayed as I was told these older machines didn't always refresh fast enough to show the change.

I've read older threads on tapping, some of them helped me some didn't but haven't been following the forums much lately. This time of year I spend more time on the tractor and in the barn than inside so I'll need to search for recent threads concerning tapping over the holidays. Problem is there is a lot of assumed knowledge that is never really discussed in a lot of these threads and as I have so little experiance and have been working by myself for the vast majority of it I miss somethings and rather than hijack someone else's thread... The only real foundation I have in machine tapping is power tapping on manual machines which is always slow rpms so maybe I'm trying to correlate apples to oranges?

Thanks
Scott

Do you mean you use 40% of 80sfm for tapping? In other words 32sfm which is 34% of 93.75sfm or 341rpm???

If you are running at this rpm that could be the reason for breaking taps.

I have found with tapping just about any material that sometimes the chips form nicer when the tap is running faster; they seem to peel off in nicer curls rather than folding up in the fluts and jamming.

Also on the MiniMill I have found that when the spindle is running down below 400 rpm it loses torque and seems to have difficulty maintaining synchronization. Down in the 200 region you can sometimes hear the spindle speed oscillating. I suspect breakage could occur at slow speeds because the synchronization is lost during reversal.

This was discussed, I think, in a recent thread; have you gone through any threads about tapping?

[Geof]

..... This time of year I spend more time on the tractor and in the barn than inside..... The only real foundation I have in machine tapping is power tapping on manual machines which is always slow rpms so maybe I'm trying to correlate apples to oranges?

Thanks
Scott

I seem to spend more time in The Barn than other places (except when I am on a vacation like the last two weeks). But my barn has a Super MiniMill and a TL2 although before we bought this property it housed five horses.

You are not really comparing apples and oranges. With a proper tapping holder it is possible to tap on manual machines at hundreds or even over a thousand rpm. We had dog clutch holders which would freewheel when you pulled back so you could stop the spindle and then they had a ratchet so when you reversed the spindle they would not turn backwards so the tap would retract. It used to be impressive tapping in a big turret lathe where you would reverse a ten hp motor by simply throwing it into reverse while the machine was running 1500 rpm forward. The electric supply needed to be able to handle a 250 amp surge for about half a second while the motor was stopping.

[jybute]

If you end up milling the thread, use a solid carbide thread mill. You will have much better tool life than a tap, and if you do it correctly, faster than a tap as well. Try this cutter from Iscar.
MTEC 0250C07 16-UN (DIA. .236"Ø X .66 thread length)

[Shotout]

Geof
Ah vacation, that explains the missing persons report I saw posted yesterday. I guess I should have stated that as far as tap holders go it is either a standard collet or jacobs chuck in the shop for manual or CNC. If I tap this I'll get them to order a er-32 tap collet for that size tap, as on the CNC mill I tend to use a keyless chuck to hold smaller taps. Adds to the intial tooling cost but at least it isn't a perishable item like taps and cutters.

Jybute,
I'll check out that thread mill on Iscar's site. I'll have to compare the intial tooling and time and see what is going to work out the best for the company. This job starts in a couple of weeks so I need to be ready one way or another.

[tturnbull50]

Try this I use it on fanuc O-m +18 both vert. and horz.
You only need adjust first 6 lines of :4000 it takes care of cutter comp.

T1
M6
G0G54X0Y0S2000M3
G43Z100.H1M8
M98P4000
G0X50.
M98P4000
Z100.
M30

:4000 (THREADMILL)
#100 =-62.(START DEPTH)
#101 =10. (RADIUS OF THREADMILL)
#102 =42.(DIAMETER OF THREAD)
#103 =150 (FEEDRATE)
#104 =2.(THREAD PITCH)
#105 =12.(TIP LENGTH)
#102 =#102/2.
#102 =#102-#101
WHILE[#100LT0]DO1
G1 G90 Z#100 F500
G1 G91 X#102
G3 G90 I-#102 Z[#100+#104 ]
G01 G91 X-#102
#100 =[#100+#105+#104 ]
END1
G0 G90 Z10.
M99

[lynn mynatt]

Try this instead:
http://www1.mscdirect.com/CGI/NNSRIT...MT4NO=71325734

[sinha_nsit]

If tap breaking in deeper holes is a problem, you can try peck rigid tapping. You only have to add a Q-word (peck length) in the standard G74/G84 tapping cycles.

[Superman]

This is a 2 year old thread
I think Scott has finished the job by now

[sinha_nsit]

Sorry!!!
I did not realize that.
But there might be some people who do not know that peck rigid tapping is possible on their machines.

[Shotout]

Sorry!!!
I did not realize that.
But there might be some people who do not know that peck rigid tapping is possible on their machines.

@ sinha True enough. I think there is a thread in the Haas forum from 2006 or so where Geoff was helping me find the parameter on a TM-1 to turn on so I could do that in 304 SS. It worked well. Hey Geof, thanks a million again for all the great advise over the years, same to Derstap, Hu and the rest of you too :cheers: (group)

@Superman. Finished, changed jobs twice, got married, had a daughter, finished a degree, went from student to supervisor/floor programmer to Manufacturing Engineer @ an aerospace shop and loving life

[Geof]

It is interesting to read posts made years back when you have absolutely no recollection of having made them.

[Shotout]

It is interesting to read posts made years back when you have absolutely no recollection of having made them.

I'll be honest it is interesting to see the types of questions I was asking a couple of years ago.

[Geof]

I'll be honest it is interesting to see the types of questions I was asking a couple of years ago.

Yes!!! Once you gain experience you wonder why it was so difficult to understand back then. I have used the corollary of this when I have a hard time figuring something out or learning something new; I am confident if I persist this too will be simple just like all those other simple things that used to be difficult.

Currently I am applying this philosophy to learning golf. I had never swung a golf club until March of this year when I started lessons. I have been told numerous times that a stiff old guy like me can never expect to progress much beyond the mediocre level because it takes years and years to become a good golfer. I intend to prove that this stiff old guy can become a good golfer; just give me a couple of years.

[Shotout]

Yes!!! Once you gain experience you wonder why it was so difficult to understand back then. I have used the corollary of this when I have a hard time figuring something out or learning something new; I am confident if I persist this too will be simple just like all those other simple things that used to be difficult.

Currently I am applying this philosophy to learning golf. I had never swung a golf club until March of this year when I started lessons. I have been told numerous times that a stiff old guy like me can never expect to progress much beyond the mediocre level because it takes years and years to become a good golfer. I intend to prove that this stiff old guy can become a good golfer; just give me a couple of years.

I use to play a bit when I was younger, but the broken clubs got to be to expensive Don't tell me you are going to retire?