Need Help!- 1 metre long Internal Threading..Any ideas ??

[intelsingh]

We have jobs which require internal trapezoidal threading of dimensions 100 mm x 12 mm pitch. The threading length is 1000 mm.

Any ideas on achieving this?

[Geof]

Yes, but it will need a big manual lathe with about 3000mm of travel between centers; let me see if I can describe my idea well enough without pictures.

But first I have a question; are you working with pipe or tube that already has the hole through it? I cannot think of any easy way to bore the hole in solid material.

For the thread:

Fabricate a large fixture bolted to the saddle that can hold the workpiece and align it parallel with the spindle axis with the 100mm hole on center.

Mount a piece of round bar about 80mm in diameter and about 3600mm long in the Chuck at one end and the Tailstock Center at the other end, and also put a Steady Rest about 200mm away from the Tailstock end. The saddle has to be able to travel about 2100mm between the Chuck and the Tailstock.

At the center of this long round bar you mount the threading tool in a hole through the center of the bar. The hole for this tool has to be blind with a fine thread setscrew at the bottom and some clamping setscrews so you can adjust the tool using a setscrew behind it pushing it out of the hole.

The thread cutting sequence is:

Start with the workpiece near the Chuck and adjust the tool so it will take a cut a fraction of a mm deep.

Engage the half nuts and jog the machine so that all the backlash in the leadscrew drive is taken up.

Start the machine and take the first cut.

Stop the machine when the cutter is clear of the workpiece.

Loosen the tool and retract it so it clears the hole.

Disengage the half nuts and move the saddle back to the start position.

Re-adjust the tool to a slightly deeper cut and repeat the cut.

Do this as many times as needed to cut the thread.

Comments:

If you are working with something like DOM tube you may get a lot of chatter. It may be possible to dampen the chatter by wrapping lead strips around the tube but you may need to use a roughing tool and finishing tools to reduce the width of the cut. The reason I suggest both a Center and Steady Rest at the Tailstock end is for reducing the chatter from the toolbar; the Steady Rest adds a lot of rigidity.

Also if you are using DOM tube you may find it distorts a lot when the stresses in the tube are relieved unevenly by cutting a deep thread.

[intelsingh]

Dear Geof. Thanks for your prompt reply. I am amazed of how quickly you came up with a solution quite similar to ours, as we took almost a month to develop this job.

I was wondering whether it would be possible to get it done on a CNC Lathe of that size.

I am working with a EN:41B tube. Have done the boring and its ready to be threaded internally. I have made a sample job for my client but need some more ideas to reduce the time

Presently, I am using a 3 metre manual lathe and as you said I have already fabricated a fixture which is mounted to the saddle on which I have mounted the tube, aligned it with the center. So the tube is fixed and the boring bar is as you described. I haven't used a setscrew for adjustment of the tool but i can try that. I have to remove the tool after a cut and then jog the saddle back for another cut. I have a 'V' tool mounted at the center of the boring bar.

I was facing some problems due to chatter initially but i have fabricated a pair of fixtures which has 4 brass tipped screws which i have attached on the ends of the tube.It has 4 jaws from which i can tighten the screws so that it touches the boring bar. By doing this it has reduced the chatter but when the tool reaches the center of the job it still chatters. I have made two rings giving it some allowance in the bore so that it just lightly touches the boring bar.It is made of brass and I shall mount these under the screw tips as it will give better stability than just 4 points of the brass tipped screws. Yet to try that out.

Any other suggestions?

Do you think I should get a big tap manufactured for finishing as the client requires a 1.6Ra finish?

I am facing a lot of problems with the chips. Initially we tried to clamp a shoe, behind the cutting tool, made of softer material but chips used to get stuck due to that.
After every 3rd or 4th cut i have to remove the boring bar along with the job and then clean the insides of the job and then re-clamp it. Any ideas?

[jjobezo]

I was thinking that a custom tap could be made then use a long extension.

[Geof]

I am very doubtful that a tap would work because the torque required to drive the tap would be very large.

To try and stop chatter how about something like an 'inside-out' box tool or travelling steady? Are you familiar with travelling steadies for turning long shafts on center lathes or box tools for turning down long bars on turret lathes? You have three points of contact; the tool bit and two pads that are at 120 degrees from the tool. The pads can be adjusted so they contact the work either just ahead of the tool or just slightly behind the tool; when they are slightly behind the ride on the newly machine surface and this can sometimes by better.

For boring I would think arranging the pads so they rode behind the tool would give the best results and two steady pads would be needed.

For threading I think three pads arranged so they rode on the ID of the thread, the part that the tool does not touch; this way you would not need to adjust the pads at every cut, just the tool. Also for threading have two sets of three pads, one set ahead of the tool and one behind.

Make the pads out of carbide with the end ground to a radius to match the ID of the tube and just keep plenty of lubrication on them. If the pads make really even contact with the tube they should sweep chips aside not ride over them and cause tearing and jamming.


I don't see how you could do it fully automatically on a CNC lathe because you would have to figure out some way of automatically retracting and advancing the tool; that would be a challenge.

[BobWarfield]

Line boring setup, eh?

For chip evac, I'd make a clamp on fitting for one end of the workpiece and blow high pressure coolant down that end. It may leak like a sieve, but if you can get some volume going down the length it should carry away the chips. The trick is what sort of seal on the tool. Again, it need not be coolant tight, just tight enough so the easiest place for the flow to go is down the length of the tube.

I would take the opportunity making the coolant fitting to have it steady rest the tool bar. I would also support it at the other end of your workpiece 2, using 2 steady rests. That way you have only (!) 1m unsupported.

You can buy a high pressure setup for a gun drill that might be modifiable. See this thread for more:

http://www.cnczone.com/vb...he-192962.html

Alternatively, this seems like a job an EDM could do provided it's a sinker with enough clearances and the right axes to rotate the electrode as it is sinking. Probably have to do some custom work to the EDM, but the manufacturer should be able to advise on that.

It's not going to be fast, but it could be automated I would think.

Best,

BW

[juergenwt]

Geof gave you some very good advise. Make sure you have a hole in your bar that fits your tool bit. Round with a flat for a set screw on top. Use HSS and do use a roughing tool. Use a good cuttin oil. You may want to think about having a bar with two tool bits, cutting edge on center, 180 deg. and one half pitch offset. Can be done and would reduce chatter. Holes must be jig bored and bits precision ground.
Started thinking some more about this. I think I would go with two round 6mm HSS tool blanks and grind the thread form on center with a backup front and sides. Than I would grind a flat on top at at the helix angle of the thread.
On the bar I would add a second set screw on top. This would locate the flat on the tool bit.
1. Set both bits to the dia of the bore.
2. Lock the screw(s) on the flat.
3. Snug up the back screw(s) to the bit.
For the first cut:
1. Loosen the locating screw(s) but keep it snug.
2. Advance the backup screw(s) a small amount by turning an allen wrench a set amount (set up an indicator so both bits are on the same dia.)
3. Take your first cut from left to right.
4. At the end - remove both bits and return the compound.
If you have a metric Thread dial you can disengage the split nut, if not keep it engaged and power it back.
5. Re-insert the bits and snug the locating screw(s) up against the flat.
6. Advance the back up screw(s) pushing the bit against the indicator for a reading.
7. Lock the locating screw(s) and take your second cut.
Repeat.

[intelsingh]

@jjbezo : It is possible to make a custom taps of larger sizes than the standard ones available. I would have to make a set of Shell taps which include roughing, semi-finishing and finishing. All that I am worried about is whether the machine has enough torque to push these taps through the job. If i can achieve the same thing with a single point cutting tool, which is what i'm presently using, it would reduce my cost.

@Geof : Yes I am familiar with traveling steadies but i didn't get your point about using a box tool. Is it similar to this article http://en.wikipedia.org/wiki/Tool_bit#Box_tool , under the heading "box tool".
For chip removal I was also thinking of designing spiral shaped strips to mount over the OD of the boring bar. Something like a chip auger. I haven't tried that yet.
Doing it on a CNC Lathe would definitely be a challenge but I'm thinking of ways to reduce time and overall cost since it is a development job.

@Bobwarfield: Yes. It is a line boring setup for threading on a manual lathe. For clearing chips I wanted to try clamping a round brush on the OD of the boring bar when its in non-cutting (retracting) mode. Thanks for your ideas, i might have to get a high pressure air/coolant system for the chips.

@juergenwt: Presently the boring bar has a square cut in the center as the HSS tool is square shaped for clamping. I was thinking of threading with two tools, offset with one pitch but the problem is to maintain that with each and every cut as i don't have an arrangement to increase/decrease the tool depth. I have to remove the tool after each cut and let the saddle go back to its original position and then insert the tool again and start with a new cut. But using two tools is definitely a good idea. I'm giving it a deeper thought.

[Delw]

Are we talking almost 40" long and a 4" bore..

just off the top of my head why dont you make a tap using threading inserts. out of a bar that is slightly undersized use the inserts to adjust or set your make shift tap.( probally 5-6 of them set up in roughing and finsih configuration)

have a hole in the modified bar that will slip fit a bar holding on the back of the head stock of the machine this will keep the tapping bar semi centered as it goes into the tubing. keeping the cutting bar and tubing centered.

heres a rough drawing.and you would need a manual machine with a hole through the head stock.
the pink color is the centering bar that you would have to modify on the back of the head stock someway, should be faily simples. the blue is the part your threading and the green is the make shift tap. red being the inserts.
looks crude best I could do in 15 mins lol, but something like this I am thinking would be your best bet and your pretty much single pointing

if you cut the thread slightly undersized then you can make a plug guage with a split in it and lap the threads to a better finish and to proper size., the split ring will allow you to expand the plug gage slightly, kinda like an adjustable die but in reverse. use 06 for the plug guage and a good lapping compound.


Delw

[Geof]

Originally Posted by intelsingh ...@Geof : Yes I am familiar with traveling steadies but i didn't get your point about using a box tool...

I was trying to draw an analogy and maybe confused the issue. A box tool supports a long thin workpiece externally one three points; one is the toolbit and the other two are sliding pads. I was suggesting having three internal supports with one being the tool and two sliding pads ground to match the inside curve of the tube.

If I understand correctly Delw is suggesting something a bit similar but he is suggesting multiple toolbits; more or less a multiple insert tool tap. The problem I see with this is the possibility of the toolbits grabbing. On a regular tap the body behind the cutting edge acts as a guide; there is very little clearance here, none at all unless it is a form relieved tap, so there is heavy rubbing which tends to keep the tap centered.

It certainly is any interesting challenge.

[wildwestpat]

Might be worth while placing the thread form cutter so that it advances into the work at half the thread form angle and not square on. This will cut thread on one edge of the thread as it is being formed and will reduce chatter considerably.

Also on big threads it is some times a good idea to use a hand chaser adapted to be held in the boring bar to finish the thread. The inserts from a 'coventry'\style die holder might be adapted if the back edge of the individual cutter is removed to just leave the thread form as a thin edge with which to cut/polish the previously formed thread for the final cut.

These are observations from cutting smaqller threads on thin wall brass tube with out the use of an external jig to support the tube.

Good luck - regards

Pat

[BobWarfield]

Now you got me thinking.

Using threading inserts as the "teeth", I wonder if it is possible to make a tool that will cut the thread in one pass. At the very least, that ought to speed you up considerably.

The sort of tool I am envisioning would stagger the inserts so that each one is cutting slightly deeper than the one before. Obviously it would have to be made with some precision so everything meshed properly.

Assuming you can get to full depth of cut, the tool could even include a collar with a male thread to help provide support up inside the hole. Said collar should be more of a "chaser" than any kind of tight fight, but it ought to help support the tool I would think. It would need to be keyed or otherwise solidly attached to the cutter.

The collar could probably also conduct the coolant. I would run some small copper lines to it and situate them around the periphery.

The more I look at it, the more I think EDM is the way to go. Here is some interesting info:

http://www.edmtodaymagazine.com/Aind...6/TechTips.pdf

If you can find a machine with the right travels, their method would make it easy to modify said machine to cut your threads.

Cheers,

BW