Threading On A Lathe

[robk]

This is the 1st time that I'm doing this...

The machine is a Johnford HT-40CX-2D with Fanuc 18i-TB control.

The internal threads (6.665-12 UNJS)are in a nickel part.

 

This is a sample of the code that got sent to me, and I'm having a difficult time breaking it down, because the machines don't have any decent programming manuals.

 

.

.

.

.

(--)

(CHECK .01 STOCK)

(CHANGE INSERT IF NEEDED)

(--)

N7485 G97 S90 M03

N7490 G0 X6.3919 M08

N7495 Z5.0

N7500 G71 X6.663 Z4.000 B60 D.005 U.002 H.0761 F1 J12 M22 M73 M32

N7505 G0 Z20. M09

N7510 X25.

N7515 M05

N7520 M00

(--)

(CHECK .005 STOCK)

(CHANGE INSERT IF NEEDED)

(--)

(FINISH LV0.0 STOCK)

(--)

N7525 G97 S90 M03

N7530 G0 X6.3919 M08

N7535 Z5.0

N7540 G71 X6.668 Z3.910 B60 D.002 U.002 H.0761 F1 J12 M22 M73 M32

N7545 G0 Z20. M09

N7550 X25.

N7555 M05

 

 

Here is a sample from mastercam using longhand

 

.

.

.

G0 T0202

G18

G97 S90 M03

G0 G54 X6.3919 Z5.033

Z4.6824

X6.63

G99 G32 Z3.91 E.08333

G0 X6.3919

G0 Z20. M09

X25.

M05

M00

(--)

(CHECK .005 STOCK)

(CHANGE INSERT IF NEEDED)

(--)

(FINISH LV0.0 STOCK)

(--)

N7525 G97 S90 M03

N7530 G0 X6.3919 M08

Z4.6494

X6.668

G32 Z3.91 E.08333

G0 X6.3919

Z4.6824

Z5.033

G28 U0. V0. W0. M05

.

.

.

 

 

There is a total of 10 rough passes prior to the samples above.

In the operators manual they have a vague sample of using G32 for thread cutting, but they show 'F" instead of "E" for pitch...

Could anyone show me some code that works? I'm affraid of messing them up and I only have one shot.

Thanks.

[DavidSV]

Do you have to use a canned thread cycle? We always use the box format for most of our threads. They look like this:

 

O2105 (T-1)

( MASTERCAM X 01-30-08)

( T3 THREAD TOOL )

(THREAD)

N3 T0303(THREAD TOOL)

G97 S1000 M03

G00 X.29 Z-.3516 M08

G99

G92 X.2435 Z-.62 F0.03571 M24

X.2371

X.2306

X.2242

X.2178

X.2113

X.2113

G00 X.29

M09

G00 X6. Z6.

M30

 

From the G92, x is the depth of the first pass, Z is the point where the thread pass stops F is the feed rate and the M24 of our machines is a code to make it pull out faster. Each following X is a thread pass at each depth.

[jeff]

quote:

---

G71 X6.663 Z4.000 B60 D.005 U.002 H.0761 F1 J12 M22 M73

---

B=Angle of thread

D=D.O.C. of thread per side

U=Stock to leave in X for finish pass (per side)

H=Height of thread per side

F=# of finish passes(a guess)

J=Brain fart,can't remember

M22 AND M73 Have to do with chamfering on/off I believe

 

You can use G32, that's just each cutting pass on it's own line.

However I prefer a canned cycle for threading.

[robk]

David, where is the "X" retract distance between each pass?

[CNCGUY]

Rob,

 

Should retract to the start point. BTW - Its an internal thread. I had to look for a bit to see it myself.

[Allan]

On a fanuc:

G71 = canned roughing cycle no good for threading

G70 = canned finishing cycle no good for threading

G76 = canned threading cycle

G32 = box style threading cycle (no support for taper thread) and you need to program the retract and rapid to front of part.

G92 = Box threading cycle (no support for taper thread) returns to start position and remains modal untill canceled by a G01 or G00 depth cuts are just X values.

Fanuc should support the E for feed rate, the E value is good to 6 decimal places (usefull for threads where accuracy is important like 18TPI E.055555)

If the E gives an alarm use an F in it's place.

 

Hope that helps

 

Allan

[robk]

Thanks Allan.

Could somebody please break this down for me?

I don't know the meanings of P's & Q's in the sample below. I am thinking that R is the amount of stock left.

 

N20 G97 S90 M03

N21 G0 X6.3919 Z5.033

N22 Z4.7494

N23 Z4.75

N24 G76 P000060 Q0 R.001

N25 G76 X6.668 Z3.91 P381 Q371 R0. F.08333

N26 Z5.033

[3rdstring]

First Line

 

P 1st 2 01-99 Fin passes

2nd 2 chamfer 00-99 = 0-9.9 * lead

3rd 2 tool tip anlge, 80, 60, 55, 30, 29, 0

Q min depth of cut

R Finish alowance

 

Second Line

 

P Depth of thread (radial value)

Q Depth of first cut (radial value)

R Difference of thread radius (tapered threads? 0=straight thread

F thread lead.

 

HTH

[Tim Johnson]

N25 G76 X6.668 Z3.91 P381 Q371 R0. F.08333

 

The P381 is actually .0381 It can also be P0381. Same with the Q. You don't have to have a decimal point with any address in Fanuc and in some places (such as the P & Q) you can't have any. X-5 would read as X-.0005

[robk]

Thanks Chuck & Tim... That's exactly what I was looking for...

Now one more question... How do I know that I won't cross the threads after changing the insert and running a finish pass? Which command tells me that it has synchronised the spindle with the tool?

[Allan]

There is no sync command, it's all about where you start from in Z. To do a double start thread you start 1 pitch away in Z from the first cut.

 

Allan

[Tim Johnson]

The syncing is done from the original Z position. If you make a Z offset change between cuts You will crossthread. You can make a X offset change though. If you just change inserts you'll be just fine.

[robk]

Here is my program... When I pull away to change/check on the insert and restart the cycle the threads get crossed.

I could make the Z be the same between the 1st & the 2nd pass, but that would not give me the 29.5° lead-in.

I have tried the same thing with 0° lead-in, so the Z value is the same, but the threads still get crossed.

Help... I'm running out of scrap to practice on.

DO I need to do the whole thing in one shot???

 

 

quote:

---

(--)

N090 G18 G99

N095 M46

N100 G97 S100 M03

N105 G0 X6.392 Z5.033

N110 Z4.7668

N115 G76 P000060 Q50 R0.

N120 G76 X6.929 Z3.91 P360 Q50 R0. F.08333

N125 Z20.

N130 M00

()

(CHANGE INSERT IF NEEDED)

()

N135 X6.392 Z5.033

N140 Z4.7494

N145 G76 P000060 Q0 R0.

N150 G76 X6.931 Z3.91 P370 Q370 R0. F.08333

N155 Z20.

N160 M00

()

()

N165 X6.392 Z5.033

N170 Z4.7494

N175 G76 P000060 Q0 R0.

N180 G76 X6.933 Z3.91 P380 Q380 R0. F.08333

N185 Z20.

N190 M05

N195 M00

---

[Tim Johnson]

N145 G76 P000060 Q0 R0. << the last two digits of P is your lead in [60].

What I would do in your case is to rough with one offset and finish with another. Your leadin will be the same that way. Just make sure both offsets match in the "Z".

 

Try this;

 

N090 G18 G99

N095 M46

N100 G97 S100 M03

N105 G0 X6.392 Z5.033

N110 Z4.7668

N115 G76 P000060 Q50 R0.

N120 G76 X6.933 Z3.91 P380 Q50 R0. F.08333

N125 Z20.

N130 M00

 

N135 X6.392 Z5.033

N140 Z4.7668

N145 G76 P010060 Q0 R0.001 -- P01 = 1 finish cut R0.001 = finishing amount radius value

N150 G76 X6.933 Z3.91 P380 Q370 R0. F.08333

N155 Z20.

N160 M05

N165 M00

[rdkllkng]

Hey Jeff! "J" is the number of threads in one inch. This the same way Okuma does in in their OSP5000/OSP7000.

 

 

From the Undisputed KING Of brain farts!!!!

 

Terry

[robk]

I would just like to say thanks to everyone that helped me out with my questions...

Come to find out the encoder in the machine was bad

Too much hair turned grey over this matter.

[Reece L Gibson]

G32 = box style threading cycle (no support for taper thread) and you need to program the retract and rapid to front of part.

__________________

G0X.95Z.1

G32X1.125Z-.75F.0714

G0X1.25

Z.1

X.94

G32X1.115Z-.75

 

This should give you tapered threads

______________________

G92 = Box threading cycle (no support for taper thread) returns to

 

G0X1.25Z.1

G92X1.125Z-.75I-.04F.0714(Iis the radial taper amount)

X1.115

X1.11

X1.1...

This should give you tapered threads