What's new
What's new

G76 Help with strange pull out issue.

yardbird

Titanium
Joined
Jul 3, 2013
Location
Indiana
I've been trying to help someone out with a strange issue with the G76 threading cycle. I'm stumped!

The original question is below...

"Trying to get a 1/2 turn pullout on this thread and a P010500 gets me a rapid out at the pullout Z, then finishes feeding to the Z- value. Help with getting a 180deg. pullout instead of the rapid out?"

Thread kind below...

"It looks like a modified buttress, or maybe a sawtooth is a better description. Working side is 65deg, back side is 25deg, with a .125" wide flat on the root."

Code below.

G0X6.3Z.5
G76P010500Q40R15
G76X5.905Z-5.125P1500R0Q75F.625

I get the exact same thing when I run this code.:scratchchin: The only way I've been able to get it to thread all the way to the end is P**00** straight up pull out.

My thoughts are that the thresd depth being so deep is what messing this up.

Anybody see what the problem is? Can this program work with a half rotation pull at the end?

Thank You...

Brent


20180113_170506.jpg
 
Last edited:
I've only been able to get less than one turn of pull out when the spindle speed is slow enough for the rapids to have time to move the tool out.

P**00** works for me.
 
Yeah it runs with P**00** like it should.

After some more thought. Fanuc call the pull out angle at "around 45deg". To my understanding this isn't parameters dependent as in you can't change the angle.

The lead of this thread .625 and half of one rotation would be a distance of .3125. I'm thinking this is out of the range of "around 45deg" is why it pulls up short of the end but continues to the final Z depth?

Hell I don't know! I've dicked around with damn near everything, the only way it isn't jacked up is P**00**. It's hard for me to except it can't be done.

Brent
 
Last edited:
Looking in the parameter manual #5130 "chamfering distance" set via the middle two numbers of the P**00** of the canned cycle.

Parameter 5131 "chamfering angle" is this a way to change the angle at the pull out?

Brent
 
Hell I don't know! I've dicked around with damn near everything, the only way it isn't jacked up is P**00**. It's hard for to except it can't be done.
Does G33 work with your control ? Pretty easy to progam any pullout you want that way.
 
Looking in the parameter manual #5130 "chamfering distance" set via the middle two numbers of the P**00** of the canned cycle.

Parameter 5131 "chamfering angle" is this a way to change the angle at the pull out?

Brent
Hello Brent,
Yes, the angle of what Fanuc refer to as Thread Chamfer can be specified by this parameter; the setting range for which is 1 to 89degs in 1deg increments. if an out of range value is set in the parameter, the chamfering is done at 45degs. Accordingly, if the value set is Zero, chamfering is done at 45degs.

Regards,

Bill
 
Hello Brent,
Yes, the angle of what Fanuc refer to as Thread Chamfer can be specified by this parameter; the setting range for which is 1 to 89degs in 1deg increments. if an out of range value is set in the parameter, the chamfering is done at 45degs. Accordingly, if the value set is Zero, chamfering is done at 45degs.

Regards,

Bill

Hi Bill,

Would this parameter have any bearing on this issue. What's causing this cycle to exit early then continue to the final Z depth?

What's your take on what the heck is happening here? Fanuc G76 can't make this thread?

Brent
 
Last edited:
Hello Brent,
Yes, the angle of what Fanuc refer to as Thread Chamfer can be specified by this parameter; the setting range for which is 1 to 89degs in 1deg increments. if an out of range value is set in the parameter, the chamfering is done at 45degs. Accordingly, if the value set is Zero, chamfering is done at 45degs.

Regards,

Bill

Bill, can you clarify/expand on this bit?

Do you mean that Pxx00xx (which I normally use) is equivalent to Pxx45xx ?

Would Pxx01xx actually be the most abrupt pullout possible? I'm very curious to know if I've been doing this wrong the whole time!


Edit: Above is all nonsense because I confused Bill's explanation of 5131 with 5130. Follow is still true however.

Threading right up to a shoulder has always been very awkward with G76, requiring a much lower spindle speed than I'd use otherwise, or the result is the thread pulling out too far from the shoulder. The only two lathes I've used that were not Fanuc were an early '80's Harrison w/ Anilam Crusader II and a mid '80's Gildemeister w/ EPL control, and both of those could thread up to a shoulder much better than any of my modern Fanucs!
 
Last edited:
Is X6.3 your actual major diameter?
I'm looking at P1500 in your second line, why not P2000?
I'm no programming expert, so I'm just curious if this would affect anything?
 
Is X6.3 your actual major diameter?
I'm looking at P1500 in your second line, why not P2000?
I'm no programming expert, so I'm just curious if this would affect anything?

2nd P is the thread hight. Major diameter subtract the minor diameter divided by 2 is the P thread hight. That makes the major diameter 6.205 back figuring.

6.3 is I'm assuming a safe clearance diameter off the part.

Brent
 
Do you mean that Pxx00xx (which I normally use) is equivalent to Pxx45xx ?

Would Pxx01xx actually be the most abrupt pullout possible? I'm very curious to know if I've been doing this wrong the whole time!

This is my understanding of how this works.

Lets assume we're cutting a 3/4-10

P**00** = 90deg or straight up pull out. The tool will travel across until it reaches the final Z depth the rapid straight up and return to the start position.

P**05** = 1/2 rotation of the spindle, distance .050"

P**10** = 1 complete rotation of the spindle, distance of .1"

Threading to a shoulder the tool will never go any deeper than the Z in 2nd line. It just depends on how much at end do you want to be a complete thread?

Having said this I'm also a little unsure where this "around 45deg" angle comes into play.

Brent
 
Last edited:
Threading to a shoulder the tool will never go and deeper than the Z in 2nd line. It just depends on how much at end do you want to be a complete thread?

What I'm getting at is this; say I'm cutting a thread up to shoulder with no undercut, maybe an M12x1.75 for example. The shoulder is at Z-20.0. I can program the thread to stop at Z-19.8 or something like that, and have a standard nut screw right up the shoulder (the chamfer in the nut is big enough to clear the unthreaded section at the shoulder).

On either of the old dinosaur lathes I'd be able to run this thread at like 2k+ rpm and it would work fine. I used to do that all the time. On any of our Fanuc lathes using G76 I have to run it at like 600rpm max or the nut won't screw up to the shoulder. Even if there is an undercut I have to run it slower than I'd like because it keeps pulling out of the thread too soon. Sometimes I've even cheated by programming a Z value slightly past the shoulder. I have tried different values in the thread chamfer thinking that I understood how it works, but now I'm not sure. Our Doosan S310SMLY for example can move ten times quicker than the old Harrison/Anilam and the 18i must be orders of magnitude faster, but for whatever reason that lathe is the worst offender for not being able to thread up to a shoulder unless the spindle is turning unreasonably slowly.
 
What I'm getting at is this; say I'm cutting a thread up to shoulder with no undercut, maybe an M12x1.75 for example. The shoulder is at Z-20.0. I can program the thread to stop at Z-19.8 or something like that, and have a standard nut screw right up the shoulder (the chamfer in the nut is big enough to clear the unthreaded section at the shoulder).

On either of the old dinosaur lathes I'd be able to run this thread at like 2k+ rpm and it would work fine. I used to do that all the time. On any of our Fanuc lathes using G76 I have to run it at like 600rpm max or the nut won't screw up to the shoulder. Even if there is an undercut I have to run it slower than I'd like because it keeps pulling out of the thread too soon. Sometimes I've even cheated by programming a Z value slightly past the shoulder. I have tried different values in the thread chamfer thinking that I understood how it works, but now I'm not sure. Our Doosan S310SMLY for example can move ten times quicker than the old Harrison/Anilam and the 18i must be orders of magnitude faster, but for whatever reason that lathe is the worst offender for not being able to thread up to a shoulder unless the spindle is turning unreasonably slowly.

Interesting! :scratchchin:

I got nothing! Unless it'd have something to do with acceleration/deceleration?

Hopefully Bill will be so kind as to come back and add to the thread?

So what is your opinion on what's happening with this thread cycle in the OP? You ever had a situation like this with a G76 cycle?

Brent
 
Hello Brent,
Yes, the angle of what Fanuc refer to as Thread Chamfer can be specified by this parameter; the setting range for which is 1 to 89degs in 1deg increments. if an out of range value is set in the parameter, the chamfering is done at 45degs. Accordingly, if the value set is Zero, chamfering is done at 45degs.

Regards,

Bill

Thank you for explaining the "out-of-range" concept.
I was always wondering why Fanuc says 45 deg when the angle is parameter-dependent.
 
This is my understanding of how this works.

Lets assume we're cutting a 3/4-10

P**00** = 90deg or straight up pull out. The tool will travel across until it reaches the final Z depth the rapid straight up and return to the start position.

P**05** = 1/2 rotation of the spindle, distance .050"

P**10** = 1 complete rotation of the spindle, distance of .1"

Threading to a shoulder the tool will never go any deeper than the Z in 2nd line. It just depends on how much at end do you want to be a complete thread?

Having said this I'm also a little unsure where this "around 45deg" angle comes into play.

Brent

The middle two digits of P, divided by 10 and multiplied by the lead, is the chamfer distance. It is measured from the axial end of the thread (specified Z). The pullout starts from this point. The pullout is always at 45 deg, unless the corresponding parameter is changed.

There are two situations now:

1. Chamfer distance is small (usual case)
The pullout consists of a 45 deg move to reach the specified Z. Thereafter, it moves radially (rapid) to reach the start radial position.

2. Chamfer distance is large (usually indicates incorrect data)
The pullout is still at 45 deg. But, before it reaches the Z value, it reaches the start X position. Thereafter, it moves axially (rapid) to reach the specified Z.

When the chamfer distance is zero, the pullout appears to be radial, but the 45 degree concept is still there.

People having some free time to read may like to read my eBook on threading for several lesser-known concepts about G76.
 
"G0X6.3Z.5
G76P010500Q40R15
G76X5.905Z-5.125P1500R0Q75F.625"

Replace R15 by R0.15 and observe what happens.
 
So what is your opinion on what's happening with this thread cycle in the OP? You ever had a situation like this with a G76 cycle?

The only times I've had G76 do weird things is when the control doesn't like the decimal / no decimal format of the Q/R addresses as Sinha alluded to.

The middle two digits of P, divided by 10 and multiplied by the lead, is the chamfer distance. It is measured from the axial end of the thread (specified Z). The pullout starts from this point. The pullout is always at 45 deg, unless the corresponding parameter is changed.

That's how I understood it. Don't mean to distract from the original issue, but do you have any ideas about the premature pullout issue that I described above?

"G0X6.3Z.5
G76P010500Q40R15
G76X5.905Z-5.125P1500R0Q75F.625"

Replace R15 by R0.15 and observe what happens.

I have a mixture of Fanuc controlled lathes, and it seems that none of them behave exactly the same in terms of whether they like decimal places there or not.

An older O-TC that I have requires a decimal point on the R address. If it's programmed without the decimal point it will cut to full depth in a single pass. The newer Oi-TD doesn't seem to care and works exactly the same whether the R address has a decimal point or not. It may be vice versa (which controls does what) as it's been a few years since I sorted this out. They all behave properly if Q has no decimal and R does.
 
... I have to run it slower than I'd like because it keeps pulling out of the thread too soon...

If my interpretation of Fanuc manuals is correct, the chamfer distance (i.e., pullout distance) is independent of rpm.
At a given rpm, the extent of inaccuracy in lead at the end of the thread , due to deceleration, may possibly vary on different machines. This is possibly the reason why the nut does not go up to the shoulder on a particular machine. I do not think it is because of a larger pullout distance.
 








 
Back
Top