G76 thread vibration

[Pauly123321]

Hi. Need help I've tried everything. I'm turning a thread 1inch1/8 by 11. 2 inches long. But it's 20 inches or from the chuck in a tailstock. Can't get rid of the vibration. I've changed speed depths of cuts ect.

 

[sinha]

Increase Q in the first block (minimum DOC) and try lower rpm.

 

[Pauly123321]

I've tried higher speed smaller cuts and then bigger cuts. Lower speeds smaller and bigger cuts. Changed the Q250 as small as Q50 I've taken out the spring cuts even the 55 in the first line. It's always squeeling on the last two cuts as it cuts full form. I've even tried truncating the thread but still no luck.

 

[Pauly123321]

I was hoping someone may have a formula of some sort where I could call up a second G76 where I can change it to a lower speed but in the same start position. So I can take the very last cut at a smaller rev

 

[tonymor]

What x value is it displaying for each of the last three cuts?

 

[Pauly123321]

I don't know now. I've finished the job and now I'm on the Colchester chasing the thread. What was you thinking?? The job will come up again in a month's time. I have no spring cuts in the cycle as its even worse. Thanks for your time to reply.

 

[Pauly123321]

Are you thinking of changing the X start position so we get the last 3 cues the same as the rest?

 

[Oldwrench]

A disproportionately long unsupported cut like that probably isn't possible without chatter.
If you can, chuck the part closer to the operation or use a steady or follow rest in a manual lathe...or...

In a CNC, start with a larger diameter (stiffer) bar, turn and chase the threads at the outer end and then turn the rest. If that bar were 1-1/2 you'd have no problems. Stiffness increases as the 4th power of the diameter, e.g. a 2 inch bar isn't 2X as stiff as a 1 inch bar, it's 2x2x2x2, or 16 times as stiff. Doesn't take much. Want to chase a 2-56 on a 1/4 inch dia part 2 inches long? Easy—start with 3/4 inch stock.

 

[Pauly123321]

Thanks for the time oldwrench. The issue I have is the costumer (South Devon Railway) supplies the material and it's already 32 diameter. Even though at each end they want 2 inch long thread they want it a continuous thread. So it can't be no miss match from start to finish so we can't do it in 2 ops. I've put a request in for a traveling steady and I have more chance of getting a date with Jennifer Aniston than getting that traveling steady . This job is driving my nuts around Bends.

 

[HuFlungDung]

Can't you just write out the complete thread cycle with G33 (or whatever you'd use for a single pass)? Don't take a final pass with full tool engagement, just one side, or the other. I often do this on manual thread cutting, works well. The tool nose has to be narrower than standard, of course, so choose the appropriate insert so that you have room to manoeuvre from side to side.

 

[Pauly123321]

I'm not sure if we can use G33 we have two line G76 and we can take side cuts if we put in G76 P000055 Q150 R.05. The 55 is the infeed. It cuts in the Z and X together wich gives us our side cut and depth cut together but it won't allow us to do it in just z. I know what you're saying though. If we take the 55 out and put 00 it'll cut just like a manual lathe.

 

[doug925]

How about running your threading passes to +0.005" of final, then change your start position by .001" in Z (either way) and cut your thread again.
Or if you can G92 instead of G76, you can directly program your X values.

 

[Ox]

I'm not sure if we can use G33 we have two line G76 and we can take side cuts if we put in G76 P000055 Q150 R.05. The 55 is the infeed. It cuts in the Z and X together wich gives us our side cut and depth cut together but it won't allow us to do it in just z. I know what you're saying though. If we take the 55 out and put 00 it'll cut just like a manual lathe.

Well, for starters - dump the 55 and replace with a 60 if you can git away with the non-compliance on one side.


Then implement Flung's or Doug's ideas.



If you have a 4x lathe available, make a bronze pad to support from the lower turret.


Also - proper etiquette for threading on the engine lathe does NOT = "00".




----------------------

Think Snow Eh!
Ox

 

[Pauly123321]

Thank you doug925 I can't believe I didn't think About changing the Z by a tiny fraction. Great idea. It'll be about a month before we get another order on this job but I will certainly give it a go.

 

[Pauly123321]

G76

OX would that not change my angle of cut on the infeed though. I've not been programming long and look forward to being educated. Everyday is a school day

 

[doug925]

Yes, it would change the infeed angle.
I assume you are cutting a 55° (whitworth, or BSPP) thread.

 

[Pauly123321]

Whitworth. Interesting thought. Got my attention now. 55 Deg cutting with a 60 infeed. Would this take the pressure off of one side??

 

[Pauly123321]

Ox you're absolutely right about the 00 but in the past I've used G76 P000000 Q100 R.05 on the first line and it's sorted out vibration in the past. I don't know how or why but it's worked.

 

[Ox]

Whitworth. Interesting thought. Got my attention now. 55 Deg cutting with a 60 infeed. Would this take the pressure off of one side??

It should not rub on any of the old cut on one side, but like I said - it will be a slightly imperfect surface on that side.
Maybe you can git away with it?
Maybe not...



-------------------

Think Snow Eh!
Ox

 

[Pauly123321]

I'm with you now. I was a manual Colchester and broadbent turner for 18 years and programming for only two years now and I've still so much to learn. Thank you for opening my mind a little more.