[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.practicalmachinist.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]

...@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

[Geof]

Now you got me thinking.

The 'Orbit' thread cutting by EDM caused a bulb to light up in my head.

How many of these things are you doing, one, one hundred or more? Maybe it could be worthwile to build a dedicated machine, for which I will try to describe the operating principle.


At the center point of the boring bar held between chuck and tailstock mount a full ring of thread inserts; making this somewhat like a big thread mill with an OD just small enough to fit inside the tube.

Mount the tube between large bearings so it can be rotated, and offset the centerline of the tube relative to the centerline of the spindle by an amount equal to the thread depth.

Gear the rotation of the tube to the leadscrew so that one rotation moves the tube assembly at the thread pitch.

This device is a thread mill, the rotating cutters on the boring bar mill the thread as the tube passes over it.


If the tube offset is vertical that would allow maximum space for the chips to fall to the bottom into the space between the bar and tube; the chips are also going to be tiny because they are milling cutter chips not turnings. A good flow of coolant through the tube will readily wash these chips out.

Depending on how many toolbits are used, or if a deliberate gap is left, it should be possible to stop the cutters in such a position that the tube can be moved back to the start point with dismantling anything. This way a spring pass can be done and a very good surface finish could be expected. My suggestion earlier about wrapping the tube in lead strips to damp vibration would maybe be helpful in this system and if the toolbits were unevenly spaced and had a gap as I mention above they would not be likely to induce harmonic vibrations.

One minor problem easily fixed (I think).

If the inserts are a trapezoidal form they will not generate a trapezoidal tooth profile because the axes of the cutter head and tube cannot be offset by the thread helix angle.

However, with a bit of trigonometry that is beyond my current ability, it would (should) be possible to develop a tooth profile that would generate a trapezoidal thread profile for the particular combination of cutter OD, tube ID and axis offset.


If you cannot understand my written description send me a return airplane ticket and I will fly over and supervise construction of this machine.

Note the sentence above is a joke; I don't really have the time to flit around the world pretending to be a consultant.

[Delw]

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.

Last night I was reading your first reply and it dawned on me I needed to grab a gun reamer to try and finish a project I was working on this week. Ran out to the safe and got it had it on my desk. and was reading some threads.
a gun reamer has a pilot on it to guide it down the rifled barrel when reaming.

in thinking of this thread being a 4"dia. a small pilot would maybe cant/move unless it was very long. thats why I was thinking of something like a pilot that would run down the head stock( which what I failed to draw would have to have a guide in the pipe to be threaded as well).

The reason I mentioned single point inserts and a few of them was becuase you had mentioned a tap would take to much horse power and it would. single pointing it would not need as much horse power. but to keep it from chattering or pushing away causing massive amounts of taper it would need something to hold it up againts the I.D.

which leads to another thought. if you have a bar with ajustable bearings on it matching the I.D. lets say an inch ahead of the cutter(acting as a pilot), and on that same bar had the cutter inward of the nose of the bar/bearings it might also work.
you would probably need a cap to steady the bar in the front of the pipe as well.

would be fun to try if I had lots of time and a machine big enough do duplicate such a thing,

not seeing the print I assume you need the part in one piece, however maybe theres a way to make it in multiple pcs and fit them together then weld them on the O.D. if you had the mating part you could thread them all together weld the O.D.s then unthread them and lap them in so where the 2 pieces meet they are perfect.

kinda like thowing 2 nuts on bolt, the threads are going to match if you welded the 2 nuts together.

if possible that would be the easiest and most accurate way and fastest too.


Delw
Delw

[Delw]

What are Trapezoidal Screws? back to top
Trapezoidal lead screws and nuts are power transmission screw threads similar to the Acme series but made to metric dimensions and standards. Sometimes misnamed "metric Acme" or "metric M series Acme" Trapezoidal lead screws look like Acme screws and have the same stout thread form and the same robust and durable features as the Acme series.

Trapezoidal single start thread designations are the letters "TR" followed by the Major Diameter in mm and then the pitch in mm separated by an "X". Thus, a "TR 14 x 3" Trapezoidal thread has a major diameter of 14 mm and a pitch of 3 mm. The separator "X" is commonly enunciated as "by" so one would communicate this size verbally as "Trapezoidal fourteen by three".

One subtle but important difference between ACME and Trapezoidal thread is the flank angle. Acme threads have 14 1/2 degree flank angles (29 degrees included) whereas Trapezoidal threads have 15 degree (30 degrees included) flank angles. This means that single point tooling used to produce Acme threads both internal and external cannot be used in making Trapezoidal threads and vice versa. Users must be careful when measuring all thread features to determine whether a given specimen is Trapezoidal or ACME as the two can be easily confused. For example, 1 - 5 ACME has a Major Diameter of 25.4 mm and a pitch of 5.08 mm. It is quite easy to mistake this size for a TR 25 x 5 Trapezoidal. A visual examination would 1. One such standard is the German Metrisches ISO-Trapezgewinde DIN 103 which has been adopted by the International Organization for Standards (ISO). not be accurate enough to distinguish these two sizes - caliper, micrometer or thread comparator measurements would have to be made.


http://www.roton.com/trapezoidal-lea...=Trapezoidal#1

heres another link
http://www.marylandmetrics.com/tech/thddat16.htm
I had to look this one up,

[Geof]

.......would be fun to try if I had lots of time and a machine big enough do duplicate such a thing,

... maybe theres a way to make it in multiple pcs and fit them together then weld them on the O.D....Delw

Great Minds Think Alike or F.S.D?

This type of problem is what I used to find fun when I was a few decades younger; now I don't have the energy.

I thought about fabricating the thread by coiling a spring out of wire with the correct cross section and inserting it in the tube. The tube would have to be bored slightly over the crest diameter of the thread to allow room for the form of the thread root in the spring. The spring would need to be wound slightly larger in OD than the ID of the tube and 'screwed' into the tube much like a thread coil is inserted; then end caps could be welded on.

Friction between the spring and tube should be more than enough that the spring would not rotate but it is possible the finish and precision would not be good enough. However, lapping it to the final form with a segmented brass lap may be feasible.

[Delw]

This type of problem is what I used to find fun when I was a few decades younger; now I don't have the energy.

we used to run into problems like this all the time were I used to work and it was great fun( for me not the owners) to try and figure something out. but thats when I worked for someone and got a paycheck for 60+ hours a week. since I am on my own I don't have the time, I still have the energy cause I always enjoyed machining, it would be fun to have a job were you just go around and help machine shops get weird stuff done, I did that for a few years also as my second kinda job it was a blast, few hours at this company few hours at that one etc etc mainly programing and set-ups.

Delw

[intelsingh]

This is part of an assembly. Its a lifting mechanism consisting of 4 such nuts and smaller screws passing through it. If all goes well and I complete it in time and with the required accuracies & finish, i get do do quite a few assemblies which would last me a year. As for now i have made some minor modifications to the fixture that holds the job and have attached two bronze rings on the OD of the boring bar just outside both its openings held on 4 points with bolts supported on a fixture. I'll be using some high pressure coolant but only after each pass as there isn't any place to mount a coolant pipe either on the job or on the boring bar. So might have to insert that manually through the length of the tube, clearing the chips.
I'm gonna think about the ideas mentioned here to give the boring bar more stability during threading. I had failed with inserting a shoe behind the cutter as the chips would form a heap and could feel the saddle vibrating. I am also scared of a bigger tap getting stuck inside or causing it to break, thus shall use a single point tool for now. The part needs to be a single piece as there's some work to be done on the OD as well. I would be lapping it with emery with a screw made of softer material so that i get the required finish.

I'm gonna start work on the final tube tommorow. Hope all goes well.

[Delw]

Copper tubing and zip ties/hose clamps works great for coolant lines, you can make a notch in the bronze bushings just big enough for the tubing,and even bend the lines so they fit.

When you say lapping with emery do you mean sand paper strips? I dont see how that would be possible.
your best bet for finish and tol. is grab some 06 material cut and od thread just below the low limit of the tol. and use lapping compound, if you slot the thread plug you can open it a ways so its fits nicely and evenly. I would think the threaded plug would need to be 6-8" long, it would have to have slots in it like a thread die so it would work.
Thats how thread guages are lapped in too final tols. and we have used it on threads to clean up finishes, take to size due to taper. nothing that big however.

I would like to see a picture of this just the threaded part as it sounds interesting.

[Andre' B]

Parts like this it is sometimes possible to call up the engineer who designed it and have a PC version of a conversation that basicaly starts out ,WTF were you smoking, and ends up with you finding out they really only need about 5" of thread on each end as long as the two ends are timed with each other. And it can be done as a weldment of a center tube and the two ends which can be bored and threaded on a horizontal mill for less then half the cost.

Works best when you have some history of working with each other.