Okuma LB15 threading problem

ozbob · Dec 5, 2018

Hi, I have a green screen Okuma LB15 that has started cutting the incorrect thread pitch.

The control is the OSP5000L & I have cut many threads, both imperial & metric without issue until the other day.

I ran a 2mm pitch & over 20 threads it is about 0.7mm out of wack & when I tried a 12TPI it is closer to 13TPI

I have been using
S400
G71X25.26Z-50H2.44D.3U.07F2M22M33M74
G71X--Z--H---D.3U.07F25.4J12M22M33M74
but have tried G33 & just using a feed of 2mm, all with the same results.
The tool tracks or chases the thread spot on each pass, but the pitch is wrong. Also, the pitch appears to be progressively consistent in error

So far I have checked the backlash on Z axis (less than 0.005mm)
Programed spindle speed verse actual speed (checked with digital tacho)& got:
Programed speed 500 RPM - actual 493.3
1000 RPM - actual 992
1500 RPM - actual 1489
2000 RPM - actual 1987

Any help would be much appreciated.

Regards ozbob

litlerob1 · Dec 5, 2018

"Progressively consistent" is sort of an Oxymoron. You say there is about .07mm error, but the difference between 12 and 13 TPI is .178mm.

There is something very wrong with the second G71 line. You have F25.4 which would be either 1"(25.4mm) if expressed in MM, or 25.4" if expressed in Inches. BUT you also have J12 which is a Pitch Count for an assumed 50mm, so a 4.166mm Pitch. Please copy and paste the ACTUAL code from your text editor to here, not your interpretation or memory of it.

I have cut a Zillion Threads on OSP. I don't use all that junk code (M22M33M74). Or even the U value, Ive never had a need for it.

It would seem that a feedrate has been overridden somehow. It seems like I have come across this before....but lets work on the code first.

R

ozbob · Dec 6, 2018

litlerob1 said:
"Progressively consistent" is sort of an Oxymoron. You say there is about .07mm error, but the difference between 12 and 13 TPI is .178mm.

There is something very wrong with the second G71 line. You have F25.4 which would be either 1"(25.4mm) if expressed in MM, or 25.4" if expressed in Inches. BUT you also have J12 which is a Pitch Count for an assumed 50mm, so a 4.166mm Pitch. Please copy and paste the ACTUAL code from your text editor to here, not your interpretation or memory of it.

I have cut a Zillion Threads on OSP. I don't use all that junk code (M22M33M74). Or even the U value, Ive never had a need for it.

It would seem that a feedrate has been overridden somehow. It seems like I have come across this before....but lets work on the code first.

R

Hi litlerob1, thanks for your reply. I have only been checking with a rule over 20 threads & thread pitch gauges. 0.7mm over the 20 x 2mm & the 12TPI gauge 'rocked' in the thread when checking the 12TPI thread. I realise this is not super accurate, put it definitely shows something is wrong.

The 'F25.4 J12' is just another way of specifying an imperial thread on this control. All it is saying is cut 12 threads over a distance of 25.4m...the control does the math for feed rate.

I don't use a text editor for small one offs, I write them directly at the control or I have variable programs stored in the control which I edit. Most of my work is small batch or repair work.

I was cutting BSPP & NPT threads on this machine just last week without issue...something has changed.

It would be great if you could recall when you came across this & what the outcome was. I look forward to hearing from you again.

Regards ozbob

litlerob1 · Dec 6, 2018

I can only speak from personal experience. So I would change the feedrate command to normal

which would be F2.116.

I personally don't like doing Imperial threads with Metric values, and vice-versa.

ozbob · Dec 6, 2018

Can do litlerob1, but one of the sample G71 threading codes ( the top one) in my original post uses a straight feed of F2 (MM) & it doesn't cut correctly either.

I did try a G33 without all the M codes & it was the same.

Any idea where you may have come across this before?

Mtndew · Dec 6, 2018

ozbob said:
Can do litlerob1, but one of the sample G71 threading codes ( the top one) in my original post uses a straight feed of F2 (MM) & it doesn't cut correctly either.

I did try a G33 without all the M codes & it was the same.

Any idea where you may have come across this before?

If you take ONE cut with a G01 F2MM across a shaft, what does that pitch look like then?

Bobw · Dec 6, 2018

Mtndew said:
If you take ONE cut with a G01 F2MM across a shaft, what does that pitch look like then?

Something like that... You need to figure out if this is consistent, or random..

Also need to figure out if this is strictly a feed rate problem, or is there something funky
going on with the entire Z axis. Maybe cut some steps and make sure they are what they should
be. In other words, does the Z actually move a real inch (or mm) when it is supposed to go that
far, or is it coming up short??

Assuming the programming is correct. Get those 2 questions above answered, and it should point
you to what the problem is, or at least narrow it down a lot. Example.. Are we looking at a loose
Z coupler, or are we looking at a bad spindle encoder.

litlerob1 · Dec 6, 2018

Damnit Bob, he said it "appears to be progressively consistent"

But Bob and dew are right, you need to know if it's the exact same error over and over and how much it is, by measuring the error. Also if 10mm equals 10mm programmed distance, you don't even need to cut anything just set up a Travel indicator on the Turret. You also need to know whether the Tool is lagging or advancing ±.

In the code posted, I see S400. Double check that it isn't G96S400 but needs to be G97S400!! okay.

There is a Feedrate override User Parameter, it's expressed in increments of 10%. Factory sets it to 200%, so that the knob can be utilized. I suppose it is plausible that someone changed it to 90%. They would be, what we here in America call "jack asses".

R

ozbob · Dec 7, 2018

Ok, did some more testing today. Used gauge blocks & dial to check Z accuracy & it is spot on over 150mm.

Definitely programmed in G97 constant RPM
My wife & I are the only people who use our CNC machines so no change of someone changing anything.

As suggested I did a test cut over 50mm at a G1 feed of 2 mm & got 1mm error over 20 threads.
So, I tried another cut at a G1 feed of 2.05 (1 divided by 20= 0.05) and it looked real close to a 2mm lead.
I then programed a thread using 2.05mm feed & let it run full depth. It looks awesome.

Watching the block data screen when it is threading the spindle speed indicates at 288 RPM when my G97 programed speed is 300RPM.
I have checked the spindle speed with a hand held tacho & got 294 at a programed 300, so which one correct...I'm not sure.

But I may have made some headway...just got to nut out what it how its all linked.

I now convinced the issues is my spindle drive.

This is what I came up with:

At a program speed of 300RPM, data screen shown 288...a 4% difference

ozbob · Dec 7, 2018

Oops hit the wrong button

So I have a speed difference of 4% & a feed variation (from programed of 2% (0.05 is 2% of a 2mm lead)

It is pretty hard to see the drive ratio between the axis motor & ballscrew but from what I can see it may well be 2:1

The next thing I did was ran a 2mm pitch at 300RPM programed speed (288 actual) & a feed of 2.04 (2% of 2mm)
& it came out spot on.

Next I ran a 3mm pitch at the same speed with a feed of 3.06 (2% of 3mm) & it was good

Just got to work out how its all linked...or perhaps I am on the wrong track all together.

I will try some more later...its too bloody hot now.

ozbob · Dec 7, 2018

Oops again 2% of 2mm is 0.04, that the feed I used. Sorry, been a long day.

litlerob1 · Dec 7, 2018

Unfortunately, I think you are probably correct about the Spindle drive.

Meanwhile it seems like you can get through the parts you have. I can't really think of it being anything else.

R

Bobw · Dec 7, 2018

My 2 cents. That may or may not help.. Probably not.

Just some thoughts.

If the spindle is spinning slower than the control thinks it is, that would lengthen
the pitch, not shorten it. Example. you are spinning 288, the control thinks you are
spinning 300. If you programmed a thread that has 300 threads over X distance, it would
actually cut 288 threads over X distance. You would have to shorten the pitch, not lengthen
it to get to 300 threads over X distance.

Honestly, I wouldn't worry all too much about the revs not being perfect.. That's a time thing
and could be off slightly.

Now I'm going to tell you a story about when my lathe shortened up the pitch. Was running some threads
one day, 1/4-20 or something. And all of a sudden I was getting 1/4-40's... Older lathe. As far as I can
tell, the control tells the spindle drive to turn X rpms and then lets it do its thing... And then for all
feeds, threading included, it uses the spindle encoder, it also uses the encoder for the rpm display.

So say I was programmed at 300rpms, the display would read 150, and would feed as if the spindle was going
150.. but it was actually going 300....

Why did this happen. Spindle encoder. On my encoder there are 2 pickups, an inner and an outer, one of
the pickups died so it was only reading half the pulses it should have.

So... Before you go throwing a spindle drive at it $$$$$!!!. I would figure out what the
logic is.. How your control, spindle drive and encoder interact. That should help you narrow
it down further.

ozbob · Dec 7, 2018

Interesting story bob, I will investigate further. I dont understand the workings of this system but I agree...on the face of it the thread should have a longer pitch.
I have been told that the fanuc spindle drives (which is in my machine) are adjustable.
Something else I am trying to get my head aroung is that I programed a spindle speed of 515 which indicated 500 on the data display screen, and cut a thread with a feed of 2mm...it didn't work? ?

ozbob · Dec 12, 2018

Bobw said:
My 2 cents. That may or may not help.. Probably not.

Just some thoughts.

If the spindle is spinning slower than the control thinks it is, that would lengthen
the pitch, not shorten it. Example. you are spinning 288, the control thinks you are
spinning 300. If you programmed a thread that has 300 threads over X distance, it would
actually cut 288 threads over X distance. You would have to shorten the pitch, not lengthen
it to get to 300 threads over X distance.

Honestly, I wouldn't worry all too much about the revs not being perfect.. That's a time thing
and could be off slightly.

Now I'm going to tell you a story about when my lathe shortened up the pitch. Was running some threads
one day, 1/4-20 or something. And all of a sudden I was getting 1/4-40's... Older lathe. As far as I can
tell, the control tells the spindle drive to turn X rpms and then lets it do its thing... And then for all
feeds, threading included, it uses the spindle encoder, it also uses the encoder for the rpm display.

So say I was programmed at 300rpms, the display would read 150, and would feed as if the spindle was going
150.. but it was actually going 300....

Why did this happen. Spindle encoder. On my encoder there are 2 pickups, an inner and an outer, one of
the pickups died so it was only reading half the pulses it should have.

So... Before you go throwing a spindle drive at it $$$$$!!!. I would figure out what the
logic is.. How your control, spindle drive and encoder interact. That should help you narrow
it down further.

You were spot on Bob. I fitted a NOS spindle encoder & problem is fixed.

Thanks to everyone who helped out.

Regards ozbob

netsteeler · Dec 12, 2018

WOW, We just got an Okuma lathe, and it threads fine, I was under the impression f was number of leads, and you use j for the pitch. BUT the lathe ran both just fine, RE f.0625 or j16
We do a lot of ACME threads with dual leads, so we were told to use f2 for two leads, and j for the pitch.

Guess after reading this I will have to look deeper into this.

AS FOR OZBOB's problem, is the feedrate override or spindle override at 100%. It is supposed to be locked out of use in a thread cycle, but me? I look for the simplest answer first. And since it is an OKUMA, there is a backlash setting for everything in the paramaters, check those out as well

ozbob · Dec 13, 2018

netsteeler said:
WOW, We just got an Okuma lathe, and it threads fine, I was under the impression f was number of leads, and you use j for the pitch. BUT the lathe ran both just fine, RE f.0625 or j16
We do a lot of ACME threads with dual leads, so we were told to use f2 for two leads, and j for the pitch.

Guess after reading this I will have to look deeper into this.

AS FOR OZBOB's problem, is the feedrate override or spindle override at 100%. It is supposed to be locked out of use in a thread cycle, but me? I look for the simplest answer first. And since it is an OKUMA, there is a backlash setting for everything in the paramaters, check those out as well

Hi netsteeler, mine is an old (1984) lb15. When using a threading cycle feed is automatically located at 100% but spindle speed isn't. I think they will still cut the correct pitch regardless of the spindle speed setting (eg 80%) but will change the tracking if you change speed after a cycle has started.

J is not for the number of leads.
My problem was the spindle encoder...fitted a new one and all is well.

70olds · Aug 2, 2019

Just for anyone else who may come across this problem at some point. I went through almost the identical process as the OP with a used machine we bought. I could consistently cut threads if I would enter my feedrate as an "altered" pitch. I.E F1/16 would not get me what I needed but F1.024/16 would. That 1.024 constant worked with any pitch I tried. I found this thread and saw that the OP's resolution was to change the spindle encoder. I did the same, and instantly the problem was rectified. 20 minute job to replace it taking my time.

Okuma LB15 threading problem

Plastic

Diamond

Plastic

Diamond

Plastic

Diamond

Diamond

Diamond

Plastic

Plastic

Plastic

Diamond

Diamond

Plastic

Plastic

Plastic

Plastic

Aluminum

Similar threads