[tequlia]

Hi, I am looking for tooling or methods for deep hole threading.

2 1/2"-4p UNC
22" deep min.
Schedule 80 pipe 48" long
600 - 1000 pcs
Machines available: Manual TOS lathe HP not a problem
Electronic lathe manual/CNC

After being laughed at by tap manufactures and most major tooling suppliers. I am hoping someone out there has an idea. I have to match existing parts, so it can be done. All information on previous manufacture is unavailable.

Options so far: Design and build a collapsible tap based on a landis head.
Custom build a threading bar-"vibration will be a problem"

Thanks in advance.

[beege]

I think the designer didn't understand "design for manufacture". Couldn't you just thread the end for, say 3", then undercut the rest of the depth as clearance?

[tequlia]

Unfortunately requires full 22" of thread, asked for different length and interrupted. no go

[Torsten]

That Tap would pull a few horsepower to drive.
You would have to weld a extension shaft to the Tap to get it to go that deep.
I would look for the old style 3 piece Tapps for this it would reduce the force required considerably. Just have do run it through 3 times.

[Geof]

That size and that length it was probably done with a collapsing tap head but I don't know if they are even available any more so I guess you are faced with building one.

Alternatively mill it using a line boring setup in the lathe; and I guess that sounds a bit puzzling.

You are probably familiar with line boring; the workpiece is mounted to the carriage and a long boring bar is held in the chuck and supported in the tailstock. You can thread cut this way but it is tedious because you have to manually retract and then advance the threading tool in the bar because of course the bar has to stay on the centerline of the workpiece.

There was a thread recently with a guy from India doing a long acme thread this way and he was successful but it took a lot of work.

In that thread I made the suggestion to build a thread milling mechanism on the lathe. Mount a long boring bar, just over 44 inches in your case, between the chuck and tailstock as normal for line boring and have a full form thread tool at the center point; this threading tool is mounted to sweep a diameter slightly smaller than the I.D. of your thread.

Now, instead of mounting the work piece rigidly on the carriage mount it in bearings on the cross slide so it can rotate and figure out some way to gear it to the lead screw. This way when the workpiece rotates it will move past the threading tool which is rotating but not moving axially. The cut is put on by moving the workpiece by means of the cross slide.

Is my explanation understandable, it is quite clear in my head.

[Fegenbush]

Geof has the way you need to do it. You can either use a lathe or a horizontal boring mill. It would take some work, and a very stiff boring bar. The benefit of the boring mill is the rigid setup possibility for your workpiece vs using the lathe carriage. As I recall, someone had set up a micrometer type advancing tool for the tool bit on the boring bar so they could take accurate step depths.

Best of luck, and keep us updated.

[RICHARD ZASTROW]

Fegenbush is describing a set-up that was sold by Davis Tool years ago. The system was a line boring bar with precision slots in it.

The cutting tools were mounted in "boring blocks". The blocks were accurately located in the slots and interchangeable so roughing and finishing tools could be exchanged.

Because the tooling blocks could be accurately located, they could be accurately "pre-set". All that was required was bench centers and a "tenths" dial indicator.

Davis Tool was a division of Giddings & Lewis who build Horizontal Boring Mills.

I'm sure other tool manufacturers made similar devices but being from the area close to G&L (Wisconsin), the Davis line was popular here.

Dick Z

add: G&L is now part of MAG. The above tooling is still available from Davis Tool. www.maint-tech.com shown in their catalog as maintenance tool.

[BobWarfield]

I know you don't have such a machine, but EDM tapping works for that kind of hole too.

Cheers,

BW

[tobyaxis]

Hi, I am looking for tooling or methods for deep hole threading.

2 1/2"-4p UNC
22" deep min.
Schedule 80 pipe 48" long
600 - 1000 pcs
Machines available: Manual TOS lathe HP not a problem
Electronic lathe manual/CNC

After being laughed at by tap manufactures and most major tooling suppliers. I am hoping someone out there has an idea. I have to match existing parts, so it can be done. All information on previous manufacture is unavailable.

Options so far: Design and build a collapsible tap based on a landis head.
Custom build a threading bar-"vibration will be a problem"

Thanks in advance.

Find a Ship Yard or a Bridge Repair Contractor and ask them where they get their machining done. Common Machine Shops will not be able to complete this task.

[tequlia]

Thanks for the suggestions.

A normal tap is not practical because of the volume of parts. According to Taylor three to four pcs. Max before it will have to be resharpened, and backing the tap out will cause all sorts of problems with the thread due to chips.

Thanks geof. I read the thread on the acme milling. Very nice work. We have a wmw thread milling/hobbing machine for milling external threads. This could be geared to drive the tube; not being an engineer or a machinist building a powered milling bar is beyond my skills.

I have found exploded drawings for collapsible taps. the deepest on seems to be only 6" but I think i can simplify and enlarge it for my purpose.

I have tried specialty contractors for the oil, shipping and construction industries; unfortunately, we are the people they come to when they can't do a thread. LOL