What's new
What's new

Lathe out of synch for threading ?

BiltMachining

Plastic
Joined
Aug 6, 2019
Hello. I recently purchased a new lathe (Fanuc controls) and am working on our first threading project. When I thread a part the first time, the threads look great but the go ring gauge doesn't go. So I decrease the offsets a few thou and rerun the threading part of the program. The machine sounds like it is cutting threads on every pass?!?! And look at what happens to the threads (see before and after pictures). Is my spindle out of synch with my turret. It looks to be about .020 off (Z axis) when I rerun the threads.before.jpgbefore.jpgbefore.jpgafter.jpg


The G-code I'm using is:
G0 x.7838 Z.125
G76 P000160 Q010 R.001
G76 X0.667 Z-1.389 P390 Q5 F.0625
Making a 3/4-16 UNF thread.

Is my code wrong or is my spindle not synched with the turret moves ? I don't know how a thread would get generated like the "after" picture. It has happened 4-5 times and only when we run a part a 2nd time?

Thanks!
 
The majority of the times I have been asked to work on a lathe with threading problems the trouble has been with the spindle encoder or the belt driving the encoder.

Since it is (or sounds like) a brand new machine the above would be unusual, but still something to look at. Did you alter the spindle speed when you re-cut the thread?
 
Hello. I recently purchased a new lathe (Fanuc controls) and am working on our first threading project. When I thread a part the first time, the threads look great but the go ring gauge doesn't go. So I decrease the offsets a few thou and rerun the threading part of the program. The machine sounds like it is cutting threads on every pass?!?! And look at what happens to the threads (see before and after pictures). Is my spindle out of synch with my turret. It looks to be about .020 off (Z axis) when I rerun the threads.View attachment 262601View attachment 262601View attachment 262601View attachment 262602


The G-code I'm using is:
G0 x.7838 Z.125
G76 P000160 Q010 R.001
G76 X0.667 Z-1.389 P390 Q5 F.0625
Making a 3/4-16 UNF thread.

Is my code wrong or is my spindle not synched with the turret moves ? I don't know how a thread would get generated like the "after" picture. It has happened 4-5 times and only when we run a part a 2nd time?

Thanks!

your encoder is more than likely fine as it works for the 1st thread.

your lead in is a bit too close try Z0.2-Z0.5 but again your 1st run of the thread was fine so thats not the issue.

post the whole code, you got something wrong. that and you said you changed offsets as in plural, you can not under any circumstances change your "Z" offset and recut the same thread.
I am guessing code issues

if you have a problem holding z size with other tools then yes you can have a turret alingment issue, but I highly doubt it.
 
Its very strange this only happens on the rerun. My first guess would have been the part moved or two different RPM's like mentioned up ^^ there.

Your code looks ok and will run but it must take forever to do. Your first pass (second Q5) is only .0005 then you clamp it at (first Q010) .001" with a finish pass of (first R).001". Your first pass is smaller then the clamp and finish pass so something funky could be happening there. I doubt it though.

Your pull out at the is Pxx01xx is tiny and no spring passes P00xxxx. I don't know what you're making or anything about your setup but you can attack it more aggressively. Also I try to thread in low gear M41. Seems to maintain a constant RPM a little better.

Just as a reference below is my code for threading 3/4"-16 on some tool steel parts we make starting with .745 outside diameter.

Brent

N60(3/4"-16 OD THREAD)
G0G99G40G54X14.Z4.T0
T0707
M41
G97S600M3
G0Z.5
G0X.843Z.1M8
G76P021060Q0050R0
G76X.668Z-1.26P0375Q0150F.062500
M9
G0X8.
G0G99G40G54X14.Z4.T0
M1
 
Are you comping ur thread on U or W ? I have seen people accidentally comp on W and get a similar issue.
 
Not sure, but is the machine reading F.0625 (4 place decimal)? I guess being it works first time it is, but you could try E.06250 maybe and see. Also, can't change Z start point in between as others said, and second yardbird and delw with starting Z at something like .2-.5 to give it a bit more time to get a few revs before starting, just in case.
 
Last edited:
Dunno nuthin bout those fancy compooterized turnin machines, but on my VMC I can change a setting so that it does not come to an oriented stop before starting a tapping cycle. Wondering if it might have similar. Saves time, but one cannot retap a tapped hole
 
Dunno nuthin bout those fancy compooterized turnin machines, but on my VMC I can change a setting so that it does not come to an oriented stop before starting a tapping cycle. Wondering if it might have similar. Saves time, but one cannot retap a tapped hole

Retapping is possible with rigid tapping, provided the job has not been reclamped.
 
Retapping is possible with rigid tapping, provided the job has not been reclamped.

Not in all cases with a machining center. Depends on control make and machine builder and potentially the actual CNC code being used. Control parameters or builder's ladder program need to be set to do spindle orientation prior to starting a rigid tap cycle for retapping to be correct. Some builders provide a setting to enable/disable the orientation as it cuts a tiny bit of time when the tapping cycle is commanded without orientation of the spindle.
 
Not in all cases with a machining center. Depends on control make and machine builder and potentially the actual CNC code being used. Control parameters or builder's ladder program need to be set to do spindle orientation prior to starting a rigid tap cycle for retapping to be correct. Some builders provide a setting to enable/disable the orientation as it cuts a tiny bit of time when the tapping cycle is commanded without orientation of the spindle.

You are right. Spindle orientation must be enabled for rework to be possible. In such a case, the spindle stops and restarts at the R-point in a particular angular position. It is typically enabled by 5202#0 = 1 on Fanucs.
 
Yardbird -- Thanks for the reply and your program. I will change mine to your program. I'm getting more material now and will update you all in a few hours. Thanks so much for your help!!! You all know how frustrating these things get when they happen and you can't figure them out. And, yes, I'm only changing the X offset, not the Z offset.
 
Retapping is possible with rigid tapping, provided the job has not been reclamped.

uhh, not if you set it not to
[I see that has been corrected above]

when you are tapping 50 holes at 1200 rpm it saves time to not stop the spindle every time

It looks cool in clear parts to have all the tapped holes line up perfectly but no one else cares
 
If you're threading right up to a shoulder change the first P to Pxx00xx straight up 90deg withdrawal. But still check thread length Pxx10xx is one pitch worth of taper out at end, probably need to add .0625 to the Z depth to get your full thread length.

Brent
 
Big Thanks!!!! to all of you who contributed your ideas. It was an RPM difference issue between my first pass and my 2nd (rerun) pass. Before I threaded the part, I roughed/finished it using G50S600 G96S150M3. When I got to the threading tool, I changed the RPM to S600M3 forgetting to add the G97. The G96 constant surface speed screwed up the threading passes with different RPM rates. I changed the spindle speed to G97S600M3 (during the threading cycle) and all problems gone !!!!! Thanks to you all for your input. I wouldn't of thought of this without your ideas about RPMs being off. Now someone please hit me over the head with the 304L I'm threading. That was a late night of pure frustration!! Thanks again,
 
I am not a lathe guy, but I have had the same problem as OP. is this only on old controls? I would be massively pissed off if a new lathe did this!

my 90s vmcs can change spindle speed while tapping and its not a problem, why would a lathe be any different?
 
I am not a lathe guy, but I have had the same problem as OP. is this only on old controls? I would be massively pissed off if a new lathe did this!

my 90s vmcs can change spindle speed while tapping and its not a problem, why would a lathe be any different?

I'm amazed that the answer to this is not obvious.....

On your VMC, when rigid tapping, the spindle and Z both start synchronized motion from zero speed. The lathe is starting the Z motion while the spindle is turning at speed.
 
I'm amazed that the answer to this is not obvious.....

On your VMC, when rigid tapping, the spindle and Z both start synchronized motion from zero speed. The lathe is starting the Z motion while the spindle is turning at speed.

I'm not saying your wrong, but that shouldn't make any difference. I get that old stuff basically uses a "start" signal. but with modern encoders, it should be checking the spindle and axis position all the time to make sure they are in sync?

like I said I don't know the answer but I don't see why it would be any different to a VMC where you can slow the spindle or the feed while tapping and it works fine!
 








 
Back
Top