LinkBack URL
About LinkBacks
What thread is it? Are the holes blind or through tapped?
| | |
Undersize Threaded Holes After Heat Treat I have some parts that were machined with 4 threaded holes with a class 2 fit. A high tolerance job (.0002" overall stackup). These were sent to heat treat, 58-62 Rockwell C, The problem now is the holes are all undersized and cannot get the GO gage to GO. Solid carbide retapping does not work.
Does any have a suggestion to rework these parts, 240 of them?
Any and all comments will be appreciated.
Thanks in advance
Steve
What thread is it? Are the holes blind or through tapped?
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
There are two sizes, 5/16-18 and 3/8-24. Both of these are thru holes. I heard at one time about using muratic acid to retap them but don't want to test that process yet.
Thanks
Steve
I think I would try to lap the threads a bit. Use a soft bolt or threaded rod for a lap, and some grease/carborundum mixture. Run the bolt back and forth with a power tool. You might be lucky and only the threads near the surface will be distorted from the quench.
If the lap doesn't supply enough pressure, take a hacksaw and split the end for a little ways and then wedge it open with a setscrew or a taper pin. Perhaps even a roll pin driven down a hole drilled in the split end would expand it enough to allow some float to the lap.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
These parts have also been ground to size, qualified, and returned by the customer because of the tapped holes, thus the reluctance for the acid test.
Thanks again
Steve
Lapping with a bolt mounted in a reversible drill hasn't worked. I even tried diamond dust/grease solution but to no avail!
The Boss is the one that wants to try and salvadge then but my opinion it would be cheaper to make new. The time and money involved to try and rework them would be much more than making more.
I suggested that we install a setscrew in the holes prior to heat treat, but, being the penney pincher he is, well, you probably know the rest!
Steve
For parts going to heat treat we always tapped +.005", we even had metric taps that said +.005" on them hehe.
When you say carbide taps do not work, do you mean they do not open up the holes at all ?? or they bind up ??
maybe you need a bigger carbide tap ??
I think a split allthread lap might work for you ?? the lap needs to be a soft material, allthread might be just about right. I'd split it like a barrel lap, and make it plenty long, and probably use diamond lapping paste if you have it.
Another trick is one many people do not know, a carbon steel tap is harder than an HSS one, the HSS will take more heat and such, but for tapping case hardened rifle recievers carbon steel will cut what HSS will not. There are some cheapie carbon steel taps out there for sale.
Bill
Have you considered thread milling them. I know it may sound crazy but have you any thing to loose? Drop the SFPM and hope for the best!
We do several hundred parts every couple of months that need boring after heat treat to get the holes on size. 63 Rc and I had some sucess endmilling as an experiment once. It worked on a .002 (.438/.440) tolerance but the tool life was too low compared to a cermet insert on a boring bar.
The trick with thread milling would be to get the tool to chase the existing thead position. It is still damn hard material on a carbide thread mill, too.
With either rigid tapping or thread milling, it is possible that all the threads in a given hole in the part would actually be 'timed' to start at exactly the same height and phase angle, provided that one tap did all the holes (of one size) in all the parts in one setup.
I suppose the lapping action of screwing a threaded rod through the hole is not the best, since there must be clearance to allow the lapping compound to get in, and thus the pressure applied is very low and effective lapping ceases almost as soon as the lap cuts any material at all.
If a person were to machine non-helical 'threads', that is, simply cut V grooves spaced at 18 or 24 per inch in an undersize blank (essentially a toothless thread mill) made out of brass, and if said person could set up this tool and perform slow helical interpolation inside the hole, again using lapping compound as the tool spins in the threads, this lap should cut at a much higher rate.
The trick would be to set the lap at exactly the correct height to match the threads, as this helical interpolation would have to be done on a cnc. Progressive cutting could be carried out as the lap wears by either interpolating a larger diameter helix or,....advance the Z start point by a few tenths and interpolate the lap again.
While the oversize tap sounds like a simple solution, the fact would be that the hardened threads are not really very good pitch quality....sure the gauge might go, but the real thread to thread contact would be lousy unless lapping or thread grinding were used.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Steve,Originally Posted by Newby2
I suspect that the solid carbide taps were chipping because you were trying to hand tap the threads? Carbide does not like slow cutting speeds and will chip and break easily. Try a tap matic head in a drill press with the carbide tap. You will lose a few parts due to cross threading, but most of the time it should follow the previous hole. Expect to use many taps! A tap will likely only do a few holes before it's dull. You'll have to decide which is more economical, the tooling cost of rework verses just making new.
Good Luck!
Lee (Who makes threads in hard material all the time.)
Ran into a similar problem with carburized 9310 - surface was harder than a whore's heart.
Some real expensive transmission shafts that took forever to make, get splined, you know the drill.
Found a shop with a kick ass EDM guy and when he got through with them, they fit like a glove - the things were METRIC threads too.
You can probably get them photochemically milled BUT that is NOT simply dipping them in muriatic acid. This mix will etch EVERYTHING and can reall trash some hardened steels, especially steels with a lot of remaining residual stresses (as in surface ground, or subjected to high shear forces) - we learned that lesson the hard way after literally ruining some hard to get ultrafine threaded shafts
("a short muriatic acid dip will loosen up the threads, trust me .... OOPS, where'd the threads go????).
I do remember now NC thet the EDM guys could pull our chestnuts out of the fire, their edge find feature is non contact, it senses an arc jump between elctrode and part, and they can just fudge the Z until they get the biggest number in X or Y, then burn baby burn, this lines up the thread to the machine. It is faster to do than it is to type, and a real savvy guy could write a program to do it I bet, or already has.
Posting Permissions
| | |
