Chasing cast-in threads on inconel - HELP!

citizen_snips · Jul 3, 2012

My employer prepares test specimens of various exotic materials for tensile testing. These samples are 3" long cylindrical pieces, with 1/2-13 threads on each end for about 3/4 inch. These need to be chased and cleaned up for the holders of the testing machines, and they can't be just hit with a thread file - too hard.

So, we use a threading canned cycle in a CNC lathe, eyeball the first few strokes, stop and adjust in Z until it runs correctly. Then 27 strokes later, we check if it came out ok. If the threading tool was chipped partway thru, we run it again until a guage goes on smoothly.

Today I was asked to speed up. I am new, and somewhat flabbergasted at the request, since I work my butt off and try very hard to do things the way I am shown. I would love to reduce the number of strokes used, since we are not actually cutting the entire material, but simply cleaning up the existing threads.

Any thoughts, oh great and wise ones?

Armedsask · Jul 3, 2012

How much are you actually cutting? Since you say you are just chasing threads, could you not adjust your cut depth to take fewer passes? What is your current cut depth? Could you get some special inserts that would allow for heavier cuts?

I've never worked with inconel, so I might not know what I'm talking about.

litlerob · Jul 3, 2012

Inconel is tough, but chasing existing threads, I would use a Die Nut. If that isn't an option, reduce the number of passes in the program, offset the tool the amount of the approach point make sure everything is in line and offset it back down to the cut.

S_W_Bausch · Jul 3, 2012

Yeah, me too, never worked with inconel, but am wondering if a gentle notice to the customer to replace/renew the mold might be a good starting point. Make some measurements, be prepared to communicate what is wrong. Perhaps they are assuming an incorrect shrinkage?

If the problem is shrinkage affecting the threads, perhaps some custom threads for the casting company to use?

They don't know the mold is wearing? Are they are waiting to hear from your company? Either way, it seems it would be justified of your company to ask if the customer could do better. At the least, they can tell you what alloy it is, so you can research the issue (and figure out the correct shrinkage).

This document indicates a threading die, but this is Inconel 725.
http://www.specialmetals.com/documents/Inconel alloy 725.pdf

If the mold can't be remedied, you are probably stuck with the current process, though grinding the threads might be an option. Determine the specific alloy, do some homework.

From the archives: http://www.practicalmachinist.com/vb/cnc-machining/i-dont-enjoy-turning-inconel-208073/

citizen_snips · Jul 3, 2012

Thank you all for input. The most common alloy I encounter is iconel 718. Discussing the mold repair is out of the question - these processes have been in place for quite some time, and complaining will not help.

Thanks for that link, I will also look at the " I don't enjoy turning inconel" discussion after I finish responding. We use carbide inserts, and my g76 skills aren't up there yet - I am a miller trying out lathe CNC for the first time. But, it looks like we start with .001 depth of cut, and my final pass request seems to be 4.

g76 P040060 Q025 R.0008
G76 X.401 P480 Q001 P .0769

I copied this code today to research it and figure out how to reduce the amount of passes.

scadvice · Jul 3, 2012

A thought...

It might be possible to somehow float a roll threading tool...I think I would be calling some of the roll threading manufacturers. Just a thought... as I said.

Steve :codger:

Bobw · Jul 3, 2012

I know little to nothing of inconel, except that it's kind of a bitch. But like any material, it only sucks until you know it.

I do know castings, and one of the things I HATE is when they try and cast too many features into a part. It can make the
machining side of it 10 times harder than it needs to be.

I'd get my hands on that mold and get rid of them damn threads. Die grinder, JB weld, whatever you have to do, depending on the
kind of casting.

Simply just give me a cylinder and I'll give you threads.

Casting in threads that need to be eyeballed and chased, that's just stupid, and a waste of time.

EDIT: Scadvice and rolling, get a simple cylinder on the end of the specimen, turn it and roll it. Or better yet, send it out. Super simple.

citizen_snips · Jul 3, 2012

Intriguing - I have used roll taps before, but I haven't tried to roll an external thread. Hmmm.....I would love to float a multi toothed tool in on a spring or something, let it align itself by catching on the top of the threads, then add pressure and let it float down and off. Hmmm!!!

little.one.der · Jul 3, 2012

What I would do, YMMV, is use a G92.
It's a single pass threading cycle.

G92 X.401 Zx.xxx F.0769

And this is how I would do it.
Let's say you just put a new piece in the machine. Dialed it true and you want to start cutting.
Offset your threading tool THE HEIGHT of the thread.
Run a pass.
The machine will make a pass above the thread major. I hope you kept an eye on it.
When your tracking the insert (don't watch the part. Watch the insert), you can see how it lines up with the existing thread.
Step one is to offset the Z to get as close to the root as possible.
Offset in the positive direction, away from the part, if you have to thread up to a face.

So you think the insert is lined up perfect? Drop the X offset what you feel comfortable with. Maybe try half of the thread height.

Run another pass. Watch it. Adjust if needed.

Drop X offset again.

Rinse and repeat.

It takes longer to type this out than to do it.

I hope I explained it. Good luck.

citizen_snips · Jul 3, 2012

little oneder, you just pretty much described the step by step of what I do with the full cut canned cycle. Except, after I've lined it up I wait while it makes 27 passes. I will look at g92. Won't that speed me up!

I think that they have just lived with the full canned cycle, and since they use carbide inserts, they just go thru them like crazy. And with a 4 hour turn around, they stick with what they have found to work and just keep pumping these things out. I must ever so gently suggest a different process.

Bobw, we are the guys you send this shit out to!

S_W_Bausch · Jul 3, 2012

I must ever so gently suggest a different process.

The bosses won't mind if your risk achieves a reward, it's all the cowards that thought of improving the process for the last decade, and were too frightened to suggest an idea and too lazy to 'sell' an idea, they won't be happy with your success.

Good Luck
Steve

citizen_snips · Jul 3, 2012

Thank you, Mr. Bausch. Shop politics has always been hard for me - people skills far more difficult to master than machining skills.

breakit · Jul 3, 2012

Is it that the cast in roughness is acting like an interrupted cut and breaking the tip, or cast-in inclusions etc are causing the problem? I find threading superalloys that eventually a strong chip can develop and pressure the thread tool too much and cause failure.. we often just change the insert every part because the sharpness plays into that chip development.

This seems to me a strange process. Normally those threads have a quite high concentricity requirement with each other, and the center part of the sample. If you don't have that you're not going to be meeting the ASTM bending requirements. Are you turning between centers and running the 2 thread sides at least? I understand you can't change the process, but it would have been better to make blanks shaped like the final part with some extra material, rough it to a decent profile and do the threading by machining only. Then you eliminate a tough / rough surface and get the proper concentricity in a single fixturing.

citizen_snips · Jul 3, 2012

breakit said:
Is it that the cast in roughness is acting like an interrupted cut and breaking the tip, or cast-in inclusions etc are causing the problem? I find threading superalloys that eventually a strong chip can develop and pressure the thread tool too much and cause failure.. we often just change the insert every part because the sharpness plays into that chip development.

This seems to me a strange process. Normally those threads have a quite high concentricity requirement with each other, and the center part of the sample. If you don't have that you're not going to be meeting the ASTM bending requirements. Are you turning between centers and running the 2 thread sides at least? I understand you can't change the process, but it would have been better to make blanks shaped like the final part with some extra material, rough it to a decent profile and do the threading by machining only. Then you eliminate a tough / rough surface and get the proper concentricity in a single fixturing.

Oh, yes. You definitely understand what I am dong. The cast in threads are rough, and come from many molds, brining variation along with them. The concentricity required is .00125 between the threaded ends and the test guage area. We do not meet this. There is a "clause" in the ASTM stating that if it is not met, just have it in the records.

Since we do not meet this, we chase one end, turn the lil sucker around and shove it in a collet, and chase the other side. This drives me crazy, because the inconel does not like having it's threads crushed in the collet and I end up rechasing and getting this request to speed up. The other guys just send the damaged parts on to the next station, and the techs bring them back for rework. GRR!!!

breakit · Jul 3, 2012

Aiiieee. Well, I feel for you. 718 is expensive, and if you're using 718 for something, that something is most likely expensive also... normally myself I'd say better to do it right the first time in that case...

But, if it's any consolation, I'm a business owner also and know sometimes there are other factors impacting choices which from a purely technical standpoint don't seem right..

Maybe some tape over the threads could help against collet damage when doing the second side? I do hope you have a center supporting the ends when they are being threaded.

good luck!

citizen_snips · Jul 4, 2012

Yes, we use a center opposite the collet; I thank you for your input, and for feeling my pain!

Sean the Dog · Jul 4, 2012

Does this absolutely have to be done in CNC? Sounds much easier to chuck it in a manual lathe (collet?), pick up the thread, and cut it. Depth can be adjusted as you go, depending on what the material condition is.

SND · Jul 4, 2012

Seems hardly worth doing cnc to me either, would only be a few minutes manual and certainly more accurate to line it up.

jdj · Jul 4, 2012

Bobw said:
I know little to nothing of inconel, except that it's kind of a bitch. But like any material, it only sucks until you know it.
.

It is not AS BAD, once you get to know it, but it is always sucks!

jdj · Jul 4, 2012

Inconel is one of those materials that the experts tell you to HOG on. I understand why (work-hardening if you are rubbing more than cutting) but in an operation like threading, you can't really HOG. You have to find a middle ground. Adjust your threading canned cycle to take a little more off per pass (will take fewer passes also) and see how it goes. DON'T take TOO many "spring passes" either. You will only be making the material harder. Can't guarantee it will work better, but it is worth a try. Good luck sir.

Chasing cast-in threads on inconel - HELP!

Aluminum

Aluminum

Hot Rolled

Diamond

Aluminum

Titanium

Diamond

Aluminum

Cast Iron

Aluminum

Diamond

Aluminum

Aluminum

Aluminum

Aluminum

Aluminum

Cast Iron

Diamond

Diamond

Diamond

Similar threads