Help OD threads on CNC lathe - rough first couple threads

[cosmos_275]

First time cutting OD threads with my CNC lathe (2 axis Doosan 2100A). Material is 7075 Al. Threads are M16x1.0. Using laydown insert:

16 ER 1.0 ISO​

MSC part# 05766357

My training guy said don't take more than .010" per pass (radially). So, I'm taking 3 passes and 1 finish pass 2 thou depth. The first thread or two are pretty ratty looking (rough with burrs), then look great after that. Only running 400 RPM. Flood coolant. Any ideas for improvement?

 

[david n]

1.0 thread.....7075.......that Lynx can handle more RPMs..........crank it to at least 1000 rippems......... I thread at 2000 RPMs in 6061...............1.25 and 1.5 metric threads within .01" of a shoulder............and many times threads in any material will have a ratty looking first thread. Run your finish tool over it again and then a threading spring pass.

 

[DouglasJRizzo]

I would go to about 1000 rpm.
Also, make sure that the tool is about .2" away from the front of the part and at least .25" from the OD.
The reason is that the machine needs space to cut the thread. It needs to accelerate the servos and also to not clip the top of the threads.

 

[cosmos_275]

Ok, I think I have it starting out 6mm from the part in Z, not sure about X. I'll give it some more space to synch. I'll try 1000 rpm. Not sure I can do a spring pass. Fanuc I guide let me do finish pass # of times, but not sure. Will it do a spring pass if you set finish to zero? Maybe I can just make it really tiny then repeat. Thanks.

 

[DouglasJRizzo]

Something like this:

G76 P020060 Q0020 R0020 - (2 spring passes, straight pull out, 60 degree threads, leave .002 for finish, minimum cut of .002)
G76 Xxxxx (target point) Zxxxx (target point) Pxxxx (radial height of thread) Qxxxx (1st depth of cut) Fxxxx (thread lead)

 

[gcodeguy]

OP, I assume you are manually programming each pass given what you posted. That lathe should have G76 cycle available for you to use. Use it. Very, very seldom do I need to manually program a thread to achieve the desired results.

I'd be cutting 316 SS at about S2300 for that diameter. You are running super slow. Slow can look like crap. Crank it up to at least S3000.

60 degree compound infeed only cuts on one side of the insert. Hardinge tech guy told me many, many years ago that they found (thru tests) a 25 degree compound infeed to be the best overall. Closest you can get with a 2-block G76 is 29. Single block G76 you can specify a 25 degree compound infeed. I only use 60 degree when trying to eliminate chatter....after already having slowed RPM.

New lathes like the OPs should be 2-block G76 cycle.

EDIT: And as already stated, start the tool far enough away for the turret to reach the programmed feed rate. You need next to nothing at S400. You will need more at S3000.

 

[Rob L]

I do M16x1 a lot and I run 2000rpm and start the threading 3mm away from where the threaded section actually starts.

I also don't cut my start chamfer or relief cuts until I've done the threading, always find the start and end can be a bit ratty as mentioned above so doing those after just removes that whole section entirely and leaves nice threads, I then go back and run a spring pass just to clean the thread up, it's not the fastest way of doing it but it's a way that works well for me. With fresh inserts that way I get completely clean threads, once they have a bit of use I normally find a small burr on the top of the first half a thread but nothing too hard to get rid of.

Regarding compound infeed angles I just plunge cut, I've tried different angles before and noticed 0 difference, I either get nice threads or ratty ones (I'm looking at you 6082 T6) regardless, all my tooling catalogues say it isn't required for a small pitch thread like that.

 

[gcodeguy]

If you're running nothing but aluminum, then compound infeed probably doesn't do squat, and you may even get a better finish on the sides of the thread with 0 infeed. I run a lot of 316 SS bars and castings. Inside and outside threads. I find compound infeed can make a difference. A zero infeed creates the toughest chip. Small internal threads can be a pain regardless of infeed. I'd rather thread O.D. all day long.

BTW, Umteen years ago I had to run something like a .3125-8 UN in a soft steel. G76 sucked no matter what. Manually programming zero infeed and creating thread with only 3 passes yielded a beautiful thread. Not something I would have normally considered...and haven't since that job.

 

[gcodeguy]

OP. We are currently running 6061 on two lathes. TW-20 has been running the same job for 5 years or a bit more. Main spindle machines a 1-12 UNF internal thread. S2000 P000129. Subspindle is making an M28 x 1 internal thread. S2000 P000155

Other lathe rigid taps four M6 x1 holes on the sub at S1295. It makes a 7/16-20 UNF at S2000 and P000155. Beyond that is a 5/16-24 UNF at S600 and P050160 and still has faint chatter. It's a solid carbide threading bar, but due to thread size the bar is very small and is ground back to clear the 7/16-20 thread. Both internal threads, obviously.

Main spindle machines a 1 1/2-12 UNF external thread at S1500 and P000129. Slower RPM is because there is no thread u-cut and I need to get close to the shoulder. I am thread milling two 9/16-18 UNF side ports at S3000 and F.005 for the rough pass and F.004 for the finish pass. Beautiful looking threads.

Absolutely no burrs allowed anywhere including the threads. Managed to get rid of all the burrs with tools used to create the holes and threads...EXCEPT for the 5/16-24 thread chamfer. Had to add a brush to remove the last teeny bit of burr on the first partial thread.

As you can see, compound infeed is not critical on aluminum. However, the only reason I went to 60 degree compound infeed was because of chatter on the 5/16-24 thread. I also thought it might help with the burr being crated on the first thread. It didn't.

 

[sinha]

Ok, I think I have it starting out 6mm from the part in Z, not sure about X. I'll give it some more space to synch. I'll try 1000 rpm. Not sure I can do a spring pass. Fanuc I guide let me do finish pass # of times, but not sure. Will it do a spring pass if you set finish to zero? Maybe I can just make it really tiny then repeat. Thanks.

The number of finishing passes in G76 can be specified 1 to 99. Even if you specify 0, it is taken as 1.

 

[sinha]

Something like this:

G76 P020060 Q0020 R0020 - (2 spring passes, straight pull out, 60 degree threads, leave .002 for finish, minimum cut of .002)
G76 Xxxxx (target point) Zxxxx (target point) Pxxxx (radial height of thread) Qxxxx (1st depth of cut) Fxxxx (thread lead)

Actually, this will execute two finishing passes. The first pass will remove the material specified as finishing allowance. All subsequent finishing passes, one in this case, will be spring passes.

 

[DouglasJRizzo]

Actually, this will execute two finishing passes. The first pass will remove the material specified as finishing allowance. All subsequent finishing passes, one in this case, will be spring passes.

Yes! I usually do two finish passes.

 

[cosmos_275]

Ok. I got a chance to try some things. Increased passes to 6: 2-3 of which are spring (seems a lot passed to go from 16mm OD to just under 15mm minor). RPM to 1000 and increased space for it to synch. A little better, but the first thread is still a little ratty. I ended up threading some extra material and then taking another OD finish pass and remove the extra threads, so the parts look good now. I'm not sure this technique will always work, but good for now. I'm not sure how fast I can ask this machine to thread. It tops out at 6k. Too fast and it won't synch well? Thanks for al the help.

Edit:
also infeed is radial.

The control has Fanuc I-Guide, so it has "macros" that guide you through programming lots of things, threads included. So, the end resulting code looks like this:

G1140W2.C0.01K2.S1.P4.Z10.D3.L3.M0.
G1461W1.D16.Z-12.L1.M12.3H0.75C2.P1.

I believe the machine does support G76, but the I guide is nice for a newb like me.