First time doing Acme Threads on Fanuc 21i-T, Having a problem.

[assface421]

Haven't been using the Romi M27 Lathe as much as I would like, to but I got a chance to use it this week. Master cam wrote a two line G76 threading caned cycle for a 2" 4tpi Acme and it looks like this.
G76 P020014 Q50 R0
G76 X1.73 Z-5.5 P1350 Q100 R0. F.25

The control would not take the code. After messing with it every way possible, I figured out what the problem was. in the P020014 segment the 14 is not a 29 as in every other thread I have done on this machine.

So my question is, why is this happening? How can i use the proper infeed angle without the control alarming out?

Thank you for your time, any help would be greatly appreciated.

 

[drewboyer]

Just put it at 0, you really dont need to infeed at an angle with ACME threads.

 

[yardbird]

The only infeed angles available in the two line G76 cycle to the best of my knowledge are 80°, 60°, 55°, 30°, 29° or 0°.

If you still want to use 14 you're gonna have to switch the control to use the single line G76 cycle format.

Brent

 

[gregormarwick]

So my question is, why is this happening? How can i use the proper infeed angle without the control alarming out?

In two line G76 the angle is the actual angle of the thread form, not the explicit infeed angle - hence the particular selection of acceptable angles.

The only infeed angles available in the two line G76 cycle to the best of my knowledge are 80°, 60°, 55°, 30°, 29° or 0°.

If you still want to use 14 you're gonna have to switch the control to use the single line G76 cycle format.

Brent

Going by

in the P020014 segment the 14 is not a 29 as in every other thread I have done on this machine.

it would appear to be a post error. Div by two and truncate or something. For acme it should be set to 29°, but for "every other thread" it should not...

Or maybe defining the thread or threading tool incorrectly - I am not familiar with Mastercam.

Just put it at 0, you really dont need to infeed at an angle with ACME threads.

You don't need to, but 4tpi acme is a pretty big thread to plunge.

 

[drewboyer]

Last acme thread I cut was a 1"-4 about 8" long. I used an 8 pitch insert and used 5 threading cycles.

I forgot all the infeed angles for G76, it's been 2 years since I used it. All I use now is G92 and G32.

Sent from my SAMSUNG-SM-G870A using Tapatalk

 

[Johnny Larue]

Haven't been using the Romi M27 Lathe as much as I would like, to but I got a chance to use it this week. Master cam wrote a two line G76 threading caned cycle for a 2" 4tpi Acme and it looks like this.
G76 P020014 Q50 R0
G76 X1.73 Z-5.5 P1350 Q100 R0. F.25

The control would not take the code. After messing with it every way possible, I figured out what the problem was. in the P020014 segment the 14 is not a 29 as in every other thread I have done on this machine.

So my question is, why is this happening? How can i use the proper infeed angle without the control alarming out?

Thank you for your time, any help would be greatly appreciated.

try P020029....and P1350....that needs to be 5 numbers...let me check...be back in a sec

 

[Johnny Larue]

try P020029....and P1350....that needs to be 5 numbers...let me check...be back in a sec

yes the second P is single depth of thread and is always positive and 5 places...never shorten it even with a zero

formula is this....

.61343 divided by number of thread per inch....so .61343/4 = .15335

so second line P = P15335

not sure how you got 1350 outta 1533

 

[Johnny Larue]

a simple rule with first line P is most times use 55 as this covers all threads including NPT..P020055..the compound will move 27.5 degrees infeed and most all threads will be perfect....then only time to change that number is for acme...then you just change 55 to 29 and compound will move at 14.5 degrees....also try 100 RPMs....nice threads all day long...one insert...no burrs...no chatter...etc

PS...with the 55 the tip of the tool goes down the thread side and makes better threads because of this slight pressure drop by not using more of the tip with another number

 

[gregormarwick]

not sure how you got 1350 outta 1533

Because your "formula" is approximately accurate ONLY for 60 degree included angle thread forms and is entirely irrelevant to this discussion....

 

[Johnny Larue]

Because your "formula" is approximately accurate ONLY for 60 degree included angle thread forms and is entirely irrelevant to this discussion....

sorry I forgot to tell em that on an acme I add wear offset first but use that .61343 formula for all threads....but on an acme I add to offset one half of root width....that second P is just a glorified wear...it tells the control how deep to go...thats all....so first cut I have it going like .04 or so above since its 4 per inch....the acme thread guage measures at .09 root....then wire the threads...then wear offset it down required amount...this way I don't have to look at any book or chart or master cam...for all threads its .61343....and for all other threads like acme without the point....I offset first cut positive one half of the root width.....if your not gonna use thread wires and just go right to size 1st cut...then yes you are correct sir....don't use my .61343....my way will also work if you have a nut as a guage to fit....take first cut then offset it on down by .003 or whatever until it fits...hope that clarifies it

 

[yardbird]

sorry I forgot to tell em that on an acme I add wear offset first but use that .61343 formula for all threads....but on an acme I add to offset one half of root width....that second P is just a glorified wear...it tells the control how deep to go...thats all....so first cut I have it going like .04 or so above since its 4 per inch....the acme thread guage measures at .09 root....then wire the threads...then wear offset it down required amount...this way I don't have to look at any book or chart or master cam...for all threads its .61343....and for all other threads like acme without the point....I offset first cut positive one half of the root width.....if your not gonna use thread wires and just go right to size 1st cut...then yes you are correct sir....don't use my .61343....my way will also work if you have a nut as a guage to fit....take first cut then offset it on down by .003 or whatever until it fits...hope that clarifies it

Hey John,

I'm almost embarrassed to admit I'm lost! I'm sure there is a method to your madness but I can't seem to catch it. Terminology could be an issue?

P=thread hight... Major subtract the Minor divided 2 is the P. I don't understand the "Glorified wear". I believe the reason you say carry it out to 5 places is because your Hardinge goes out 5 decimal places?

Folks learn the way they were taught. I think we were just taught differently because I have some difficulty following your train of thought.

And for the record I wouldn't run the spindle to awfully fast either.

Brent

 

[sinha]

Yes, P----29 is the correct choice for ACME threads, for single-flank cutting.
Regarding depth of thread, I have a confusion. Drawing books show that depth is half of pitch. If so, P1250 should be used if the core diameter is correct in G76.

 

[gregormarwick]

Drawing books show that depth is half of pitch. If so, P1250 should be used if the core diameter is correct in G76.

That's a very rough rule of thumb that I've seen people use for metric threads.

OP's depth value is good for the thread he is cutting.