A customer brought in some stainless steel valve cages which were built very cheap somewhere over the ocean. The O.D. threads are to tight to make up and need about .005 to .008 taken off. Does anyone know an easy way to catch lead and re run these threads? the good part is that the part runs true in the chuck but the threads are 1.25MM pitch or .04921 lead and there is no room for a mistake or an undersized part:confused: . Thank You.

Do you have metric threading capability on your lathe?

If not, beg borrow or steal a geometric threading die head and metric set of 1.25mm pitch. The die heads are adjustable on the pitch diameter so they work well to create slightly under/over size threads. I would not use a carbon thread chaser on a stainless fitting. But, if you must, use anti-seaze as lube! I just don't think they are sharp enough to cut stainless let alone small amounts without riding over the top.

A word of caution if you don't already know about metric threading in an english leadscrew lathe. Once you start to pick up the thread you cannot disengage the halfnuts, or you will wipe out the threads in the next pass. This makes it very risky business if you need to rethread up to a shoulder. All you can do is back out the cutter, reverse the spindle and back the carriage up to restart the next pass.

If all you have is .002-.004 per side to remove, the thread really should be indicated in if you can rotate the spindle and gearing through by hand. Indicating the face of a machined surface first, then bringing it on pitch diameter center with a set-tru type chuck. Pitch diameter center might not be the same as the nearest non-threaded diameter. You must decide if you want to do it properly or just do it and get it done. Judging the value of the part, quality of work.....yada, yada...ya



First I set the compound at 29.5-30 deg, align a well honed single point threading cutter in the tool post, set the change gears pitch as required. I get the spindle speed very slow. Around 20 some odd rpm, engage the halfnuts and start feeding the cross slide and compound in until the right flank of the cutter touches the right flank of the thread. I zero the cross slide dial(or at least remember the position to reset later) all the while being prepared via peripheral vision of the thread ending pullout of the cross slide.

Normally I keep my right hand on the half nut lever, my left hand on the cross slide crank, prepared to pull the cutter out then disengage the half nuts, but again on metric theading I keep my right hand on the spindle clutch reverse lever. Keep in mind, big lathes take some time to slow down and reverse. Backing up a bit beyond the part to go again. Reset the cross slide to my zero point and creep feed the compound each pass until it starts to cut on the cutters left flank. I might even do a couple of passes away from the part just to get a feel for the sequence as fluid motion. No one needs an "oh $hit" panic when the cutter is in the metal.

Nothing builds your confidence like a job well done. Just as well, nothing kills your confidence more when the customer stands by and watches you scrap his urgent need!

Do what you feel gives you the best chance at success....

I'm root'n on the geometric die head if your pitch diameter is under 1"-1-1/2", but then again, doing it the hard way is the way we gain skills in the first place.....

DC

You're doing this on a CNC (turning center) not an engine lathe or a manual/cnc, right? I've had the same question on how to do it on a CNC (turning center) too, it's easy like the previous poster described on a manual/cnc or engine lathe.

I just wrote a post on how I thought you might try it but until I get the last bug worked out, I'm not posting but I think I figured it out... If anyone really knows, please post...

I've never tried chasing a part that has been reset up in a cnc lathe. The problem is always catching the original path. Perhaps this method would work.

Thread a new thread on your machine. For convenience, place the part so that the Z0 face on the new sample corresponds with the parts to be reworked. Write down the Z value of the current G54.

Stop the machine and roll the chuck over until jaw 1 is in a known position, whether it be level, or whatever, that is up to you to figure out.

Jog the thread tool over to the part. Jog the tool until it is centered in the first or second turn of the thread. Be consistent, what you use on the sample is what you would stick with on the reworked parts.

Record the current G53 Z position, if you have a display screen like that. If you have an operator display screen, you could even zero the Z display at this time.

Back the tool out. Put the first rework part into the chuck. Roll it over until the #1jaw is level again. Jog the tool down and back/forth to the put it in the center of the same thread as you used previously. Note the new Z position on the operator display. Adjust the G54 Z value by this amount. The actual adjustment amount should always be within the range of one lead, plus or minus. Do not zero the operator display again, so you can continue to use it as a measuring stick.


Another method might be to make a setup fixture, like a close fitting bushing (without any internal threads), with a heavy wall thickness. This method would only be practical if your bushing can easily contain the whole part inside. Drill a cross hole in one side of the bushing, reamed to a close fit for a piece of drill rod. Sharpen a V point on the drill rod to engage the thread. Slide the bushing over your new threaded sample, and slide the drill rod down the hole to engage the thread. You will have to slowly wind the bushing/drill rod onto the thread until the end of the bushing butts up to the chuck jaws. For this method, you will then have to mark the chuck as to the exact location angle of the drill rod.

Now, on the rework parts, screw the bushing onto the part, about the same distance as your trial part. Align the drill rod with the mark on the chuck, slide the part into the chuck until the bushing bottoms on the chuck jaws and clamp the chuck. No G54 adjustment required.

Yeah, what he said! :confused: :)

Has anyone ever seen or built a "floating" thread toolholder? What I mean is this: I was originally thinking on along similar lines as Hu on how to do it but after reading his post, I wonder how easy it would be to just buy or build a toolholder with a couple of medium duty set screws to adjust both the X and Z independently (by hand on small guides or ribs, one horizontal and one vertical) into the original thread and once you run it, lock those babies down?! All you would have to do is somehow not get your arms ripped off setting it, oh oh oh! make a blunt insert kinda tall so it would rub itself into position instead of cutting. Just make sure the set screws were just slightly snug.

LOLOL, I really doubt I explained that well at all but I should work on it after bike week in Daytona and then sell em to you guys! JK! ;) I made something similar before and after a few prototypes it worked pretty decent, only that thing wasn't intended for threading.

I used to do all this stuff manually but my left arm is paralyzed now so I actually NEED to find a way to do this accurately and reliably in a CNC. When I get the bugs worked out, I'll post pics... (Gimme six months, I'm kinda busy, plus, I usually hire my dad to chase threads, lol~)

Ok, I looked it over, I'm sure this will work with a little experimentation... If anyone has suggestions before I actually build it, let's hear em'!

The tough part in coming up with a way to resync a CNC is that not all use the same type of advance. Some use X plunge only and some use advance at a selectable thread angle.

I have often thought about a simple cutter fixture to adjust the Z position independant of the control during several cycle passes. Once sync looks ok, then Z length can be reset for the thread ending. Making any adjustments to the thread start will upset the sync again. Same procedure for chasing the next part.

Otherwise a nice software feature might be a probe capable of tracking and resyncing on its own in reference to the tool library.

DC

One,

Would you agree that despite whether or not the machine did X only or moved in on an angle, you would be lined up perfectly IF you could sync any point on any individual pass perfectly? Or would you have to then know which pass you were on and trig out the X and Z to get back to your original start point and add or subtract those values in your tool wear compensation?? (Maybe it would be only one or the other, getting late, can't think...) If I'm thinking correctly, that would be the real trick to it ONLY IF the machine in question cut in on the angle and not just a new X diameter per pass...

(I'm kinda stupid when it comes to proper terminology, lol, bear with me ;) .)

If that's the case, it's still just a matter of building the holder to self align during any particular pass. The only difference being a little bit of trigonometry involved if it wasn't the X only variety.

I believe synchronization is a function of spindle speed. Moving the start point back and forth in Z does not (should not) change the sync engagement, provided that you make the initial tool setting on a fully formed thread, not on an initial scratch pass.
I would run the full thread cycle, even on the reworks, until I was sure that the tool was safely retracting at the end of the thread. Wouldn't want to run into heavy cutting at a critical moment :)

Gotcha, I think you're right, at least on my Mori that's how it works... Thanks!

I'd expect you would need to know what type of advance the lathe was going to do, in order decide what line the sync will follow. I wouldn't think you would need to do any math in that regard.

It should be fairly simple with a good eye to get an idea where X will start cutting the existing pitch diameter. Then set the beginning or ending diameter based on the pitch height. If we are only adjusting the fixture I suggested in Z, the X should remain stable to the tool library.

I prefer cutting threads with a compound advance as in the old days. One CNC lathe I use is an EZ-Path and it does use the compound advance. If I were to set it up, I rather do it exactly as I would on a manual engine lathe and let it go from there, all be that under the lathe control. My experience has shown that making adjustments to the major diameter setting does reduce the pitch diameter at the thread advance angle. I contrived via my fixture idea, once I had it synced independent of the control, it would be a no brainer and finish the thread cycle on its own. Unfortunately, that would be a compulsory process for successive parts.

The thread sync is a function similar to electronic gearing. There is a sync pulse on the spindle and the software will move the Z in reference to the pulse feed. Commonly why it is recommended you set the thread start a few thread pitches ahead of the thread start. I have done prototype 2 lead threads in this manner. I just offset the Z 1/2 the thread pitch so the the new thread was cut in sync offset from the first. Worked like a charm at least on the EZ-Path. If I increase the spindel RPM, and recut the same part, the Z is quicker, but the sync is the same.

I have heard it suggested in other threads to move Z zero back until you achieve a resync. This takes a lot of time, but might work if others have more patience than I do.

Another method had to do with cutting a new thread the size required and then take a reference position of the spindle and Z in one of the newly created threads. Then place the part to be chased in the chuck/collet and rotated to sync its thread to the reference. Maybe this is where the floating cutter holder might pay off?

Most CNC thread reworking suggestions I have read over the years are so cumbersome, I've not tried for the sake of having other means to get it done quicker on a manual lathe.

I have racked my brains on and off the last 7+ years for a fool proof method on this. So far just a bruised brain and not much else.

DC

If you are using an newer Milltronics lathe you can use the tread chasing cycle. see the attached doc. (I had to zip it to get it to upload)
Milltronics offers a program for thead chasing that you can change the depth of cut as well but there is a charge for it.

I forgot to say the part was about 4" OD and the thread was only like 3/4" long. It has some thread relief but stops at a shoulder. I am using a Milltronics ML20 lathe with Pragatti turret so there is no way to adjust a compound. The lathe is also equiped with conventional induction spindle motor so it does not have spindle orient capabilities. I think an adjustable tool holder is a great Idea it would be easy to adjust it in to match, it just has to be ridjid, easy to adjust, and lockable. and there would have to be some sort of set up program run to sync the spindle to the part, and then adjust the tool into the thread. Thank you, The Farmer.

Perhaps thread milling might be another thing to try. This would be like a "slow-mo" version of thread chasing. I suppose the advantage would be that 'synchronization' of the thread mill can be easily accomplished with simple commands, and not the cross threading hazard associated with live threading on a lathe spindle.

I suppose chances are good that the whole batch of parts may actually be very uniform in the phase angle of the thread start, if they were all originally run on one machine. The trick would be to have good locating surfaces elsewhere on the part.

I think HuFlumgDung might have an idea. If you have a Optical comparator you might be able to layout part and thread mill and set depth of mill to match part. Not sure how to get it to run in metric though.

LJ48

What type of lathe are you doing the threading on? CNC or manual? If it is a cnc machine (and with proper software and manual operation) you can chase threads with ease. Let me know if you need any assistance.

It is CNC with handwheels and remote hand wheel atachment. What kind of soft ware would I have to have to Catch lead and repeat 3 or 4 passes to get to depth and gauge properly. Thank you for any Info. The Farmer.

Please refer to the zipped file that mholden had posted earlier in this forum. The thread chasing cycle is a one pass operation. Your machine will not be able to chase threads in multiple passes due to it not having spindle orient. The cycle is an automatic cycle where you enter all the data in one conversational page and then handwheel the threading insert into a known good thread and then hit enter and the spindle will then turn on and the machine will make a on shot thread repair. Hope this helps