O/T Please Help Me.

[TimHollis]

All our tapping has been done by hand until now.

 

The company just asked me too----

I have 20,000, 8/32 holes to TAP, 1 inch, Blind hole 1.500 deep, mild steel.

 

So the company is going to let me finally get some Tap Tooling.

 

I did do the Post search, and read them, but I'm still lost.

 

And I can’t figure out what to buy.

I am limited to getting what I need from MSC.

And having them Fed-Ex it from the States.

 

I will be doing it a Bridgeport TC1, this is a belt drive machine, not direct drive.

It does have the canned Rigid Tapping option installed. ( I have read the searched post’s, and realize the difference between belt, and direct drive)

 

I really do not know what to purchase in the way of Tool Holders.

 

The Taps I want to use. : MSC Pt# 88217385, 8-32, form tap, Thread Forming - Taps Thread Size: 8-32 Ground Thread Limit: H5 Style: Bottoming Finish/Coating: TiN Type: CNC Material: HSS

 

Should I get a-----

 

ACCUPRO

Msc# 05733191 rigid tap holder ,sys 1

OR

Accupro

Msc# 02808319 torque control tap collets

With

Accupro

Msc# 05049960 Floating tap holder

All compatible with = Bilz system

 

Or get a

msc# 00363572 Numertap BT-40 Compression 0-.250 / Tension .560 tool holder.

or

msc# 00363580 Numertap BT-40 Rigid tool collet holder

 

 

 

I did the search and I know the difference between Ridged Tool holders and, Floating Tool Holders.

 

I understand some people when tapping will Under Feed, is that what the Compression/Tension, tool Holder is for?

 

Can somebody explain to me what Bilz compatible means?

Why is everything 100/200/300 series designated?

I do have a TapMatic head, if I need it.

 

I appreciate any and all help, I can get on this 1. Even the jokes about the machine or me, as long as you leave me advice also.

 

Basically, If it were you—

What would you buy?

And why?

(remember, I am limited to MSC) there are no dealers or reps, unless I fly them in from PR.

 

Thanks

The Ex-pat

 

P.S.

I also read the Rigid Tapping Recommendations in the Instructor Forum.

But it did not help me decide which way to go.

 

[ 03-17-2003, 05:18 PM: Message edited by: TimHollis ]

[Rekd™]

I've always had better luck with rigid tapping. The floating heads are nice but prone to worries.

 

I hold my taps in a standard ER collet which eliminates the need for expensive holders.

 

'Rekd

[Toolfab]

An now to confuse you more...lol

 

We use floating tap holders here, the main reason is we use so many different types of material, floating heads allow for alittle room for error in your speeds and feeds. Basically I can be off alittle and not explode the tap! If this is your first experiance taping in a cnc, I would say go with the floating..

 

JM2C

[Surface]

Thats a lot of holes. If it were me, I would be using a tapping head regardless of rigid-tapping or belt/direct power, or what type of machine you have, and I'll tell you why.

1. Speed. A tapping head can reverse faster than your machine can. If you can save 1 second per hole, it adds up to 5 hours of machine time. A tapping head can go faster than even a specialized drill/tap machine.

2. Wear and tear. Your machine will need to go forward and reverse for each hole. Just a set of belts will cost you a hundred bucks.

 

I use a tapmatic head, but there are other brands which are good.

[Brendan P]

Believe it or not,I had problems with brand new

bought EMUGE tension/compression tap holders.

They lasted about 2 months,then started to bind.

I would defenitly buy TAPMATIC next time.

I always like to have a little "breathing room"

when tapping.

I don't think you want to "take the cheap way out" when buying a tapping head system.

[Rekd™]

quote:

---

I don't think you want to "take the cheap way out" when buying a tapping head system.

---

Especially with that many holes!

 

'Rekd

[Trevor Bailey]

There is no way I would rigid tap that many holes. Use a tap-o-matic head and still use form taps.

[TimHollis]

I want to Thank everybody who is taking the time on this one.

 

I'm still hoping for more info, Please????

 

 

Thanks

Tim H.

 

[ 03-17-2003, 08:00 PM: Message edited by: TimHollis ]

[Trevor Bailey]

Make sure that you also use a really rich cutting fluid. If you can, use some kind of oil instead of a synthetic coolant. If you must use the coolant, make it really "soupy".

[TimHollis]

I want to Thank everybody who took the time to reply.

 

I'm still looking for more, Please??

 

 

Thanks

Tim H.

 

[ 03-17-2003, 09:37 PM: Message edited by: TimHollis ]

[Brendan P]

Get yourself a tension/compression holder,program

those damn holes with the mastercam tap cycle and let her rip!

You said you were tapping mild steel......

Stop sweating it.

[Allan]

I would think that having a belt drive system would force you to use the tension compression holder, as others have stated (IMHO). Ive always had the best luck with the tension & compression holders. The go-nogo gauges were your friends!

 

 

Are these 20000 holes all in the same part? How many holes per part? if there were more than 50 holes per part, I would consider using a jurry riged tap-o-matic. Put it right in the CNC, set up a stop for the arm. You would have to do manual tool change tho.

 

 

HTH

Allan

[TimHollis]

Hello Allen.

 

About once a month I will have to run off, 2000pcs of a .250 x .250 x 3. shaft. In a 10-up fixture, for now. ( They needed them last month! 4000pc, 1st run.).

I'm hoping by next month to have a 100-up fixture.

 

ANd I have been Searching thru the Posts, reading and re-reading. But there was very little in the way of holder choice and why.

 

On the Tap.

 

MSC Pt# 88217385, 8-32, form tap, Thread Forming - Taps Thread Size: 8-32 Ground Thread Limit: H5 Style: Bottoming Finish/Coating: TiN Type: CNC Material: HSS

 

The Drill.

 

Drills Unit of Measure: Wire Sizes Size: #26 Wire, 0.1470 In. Overall Length: 3 Material: Cobalt Type: Heavy Duty Finish/Coating: TiN

 

What kind of tap would you use & why?????

What Kind of drill would you use & why.????

Under the right conditions, how long should I expect the tap should last, befor change out????

( Not counting the one's I explode!!!!)

 

I have never done this volume, of tapping in the CNC befor. And I feel like I'm in a black hole on this one. The worst part is, it takes so long to get what I need down to the DR, back on LI, I could drive over to MSC in Deer Park, in 5 min,.

 

Again Thank You, to everybody taking the time to help me out.

 

 

Thanks

The Ex-pat

 

[ 03-18-2003, 06:17 AM: Message edited by: TimHollis ]

[chris m]

Tim

 

I have a job that we run all of the time in which I roll tap #8-32 holes about .500" deep in 1144 stressproof steel and it works very well. We use:

 

Drill

 

Guhring 622 series cobalt parabolic drill. I use a #25 for the tap drill, .0025 bigger than what you have listed; you lose a little % of thread but it doesn't really make a big difference to the quality of the hole and it allows the tap to run a little more freely. I am drilling at 55 SFM (1405 RPM) with a .003 IPR feed and .600 deep with no pecks; works great for 1,000s of holes

 

Tap

 

YMW bottoming roll tap #387796BR that is TiN coated. We ran Balax for awhile and tried some OSG but this particular tap runs the best. We use rigid holders for this job but I think that a tension holder should be OK. I am running 30 SFM (about 700 RPM) on this tap and it will tap 1,000 holes without any problem whatsoever using coolant as a lubricant.

 

For your application I would definitely run a parabolic drill with maybe 2 or 3 pecks (I usually start out aggressive and break a couple of drills on a long-run job like yours) to make that deep hole and run the biggest tap drill you can while still meeting your maximum minor diameter requirements. I would also run a tension-only floating holder (if you get into compression the tap is gonna break anyway) and make sure you don't underfeed too much because a fine pitch tap in that deep hole could use up all of the tension travel pretty easily.

 

Good Luck

 

C

 

quote:

---

I hold my taps in a standard ER collet which eliminates the need for expensive holders.

---

Oh yeah, Rekd, those ER20 collets are sooooo cheap

 

[ 03-18-2003, 07:21 AM: Message edited by: chris m ]

[Smit]

If you're buying through MSC I would suggest you contact them and ask to talk with some tooling representatives. They will take a look at what you are doing and recommend a way to do it efficiently on your machine. It's what they do for a living, I expect they would be very happy to come see you. It would be a good way to get started, and once you gain some experience you can build upon that.

Smit

P.S. OK, since you're from the Dominican Republic you might have to handle it over the phone!!

 

[ 03-18-2003, 07:28 AM: Message edited by: Smit ]

[TimHollis]

Good Morning, Chis M.

 

Thank You, Thank You, Thank You!!!!!!!!!!!!

 

I really appreciate the time it took you to write that long reply.

 

This Saturday when I go to the Parquesito for an afternoon of Presidente and Bachata, with my wife, I will defiantly spill 1 on the ground for you!!!!!!

( a Good Luck Custom, performed here!!)

 

 

Thanks

The Ex-pat

 

[ 03-18-2003, 09:44 AM: Message edited by: TimHollis ]

[McRae]

I can offer my services with an onsight visit and I will bring some taps with me. As soon as you sned a purchase order and the hotel confirmation number, I will book my prepaid flight .

 

Chris has laid it all out for you in his post. My only concern is that you are going twice the depth that he is and the 8-32 is quite a slender little animal. With the hole having an extra .500 inches at the bottom, go with a long lead taper point rather than a short lead bottoming style or the intermediate plug style.

 

From the 1st edition of the "Handbook for the Metalworking Industries", Modern Machine Shop, Hanser Gardner Publications, Page 1259 Table 18 Forming Tap Drill Sizes for Class 2B Fit Unified Threads.

 

8-32

75% Thread (Theoretical Size) - .1486 close #25

65% Thread (Theoretical Size) - .1499 close 3.8mm

55% Thread (Theoretical Size) - .1515 close #24

 

With the long engagement (More than the 1.5-2 times the diameter of the screw) I would suggest to use the 55% thread diameter.

 

Regards,

[TimHollis]

Hola, Andrew M.

 

Thank You for the reply!!!!

 

This Saturday when I go to the Parquesito for an afternoon of Presidente and Bachata, with my wife, I will defiantly spill 1 on the ground for you!!!!!!

 

Change that to 2 Presidente

 

 

Thanks

The Ex-pat

[chris m]

Save all of that spillage until something actually works Tim

 

C

[Rekd™]

lol, chris

 

I was actually talking about the ER16's, but you're correct, they're not cheep, but they are on hand.

 

I must have missed this the first read through, but that #8 is going 1.00" deep! Better You Than Me!!

 

'Rekd

[McRae]

quote:

---

I must have missed this the first read through, but that #8 is going 1.00" deep! Better You Than Me!!

---

Thats why they sell them by the dozen.

[chris m]

You know, Tim, Rekd has a point there; why so much thread?

 

1) Can you counterdrill the hole for 1/2" or so to reduce the amount of actual thread depth?

 

2) Effective length on your tap may be an issue; will you need to grind relief in the shank?

 

Your best bet would be to grab a chunk of steel, throw it in a vise, and start blowing holes in it to get your parameters worked out before you try your luck on actual parts

 

C

[Brendan P]

quote:

---

Your best bet would be to grab a chunk of steel, throw it in a vise, and start blowing holes in it to get your parameters worked out before you try your luck on actual parts

---

I totally agree with you Chris on this one.

Why do you have to go 1.0" on an 8-32?

Seems a little deep for that small of a thread.

Must be engineered by G.E.

[chris m]

Hey Tim, you still ripped or what?

 

How did this work out for you?

 

C

[CPeast]

Tim Cant respond hes in teh back room hand tapping 8-32's.