ID Threading

[Toddjones]

Hi all, I'm very new to CNC and have plunged into it head first. A friend of mine is a CNC machinist however is experiance is limited in lathe work as it relates to the G Codes.

We tried to perform a simple ID threading operation but I either get an Alarm or it does something weird.

Here is the code!

%
O0800
G20
(PROGRAM NAME - XXXXX DATE=DD-MM-YY - 16-09-04 TIME=HH:MM - 17:10 )
(TOOL - 1 OFFSET - 1)
(ID THREAD - MIN. .5 DIA. INSERT - NONE)
G0 T0101
G97 S200 M03
G0 G54 X1.05 Z-2.0358 M8
X1.2688
G99 G32 Z-4. E.8
G0 X1.05
Z-2.0403
X1.2852
G32 Z-4. E.8
G0 X1.05
Z-2.0444
X1.3
G32 Z-4. E.8
G0 X1.05
Z-2.0444
X1.3
G32 Z-4. E.8
G0 X1.05
Z-2.0358
M9
G28 U0. W0. M05
T0100
M30
%

My machine does not recognise G32 and I was advised to switch it to G92. It runs without an alarm using G92 however it does not perform the operation as it is suppost to. It seems to reverse the operation. My machinist said if I try running it I will crash the machine.

I am very frustrated as I need to make parts with an ID threat.

Any suggestions would be appreciated. He advised that there are no proper Post processors for HAAS lathe's and that I believe the said the closest POST processor is MFLAN.


Thanks

Todd!

PS I hope I posted this in the right area!

[tex]

You should use G76 code because G92 is pretty complicated (needs more lines for more passes and is OK for a single pass). Just let us know the main parameters of the thread (F, M and depth in case it is metric) and I'll write you a code. It is even better if you send me an IGS STL or STP file of the part you want to machine and I'll do it with no trouble at all:

tex707@net.yu

A few more questions: which HAAS machine are you working on and what does the "E" command stand for?

I've tried to backplot your code and it looks strange...no feedrate at all?

There are PPs for HAAS lathes (by IMS) and in case you don't have one the closest match (99%) is FANUC6T.

Here's a simple G-code for HAAS lathe with FANUC controller that works fine:

N780 X47. Z1.
N790 M19 P180
N800 G97 S400 M03
N810 G76 D0.75 X59.4 Z-17.8 K2.6 F4.23
N820 G00 X47.
N830 Z1.

[kbrenneke]

O0800
G20
(program Name - Xxxxx Date=dd-mm-yy - 16-09-04 Time=hh:mm - 17:10 )
(tool - 1 Offset - 1)
(id Thread - Min. .5 Dia. Insert - None)
G0 T0101
G97 S200 M03
G0 G54 X1.05 Z-2.0358 M8
G92 X1.2688 Z-4.0 F???
X1.2852
X1.3
X1.3
M9
G28 U0. W0. M05
T0100
M30
%

Hope This Help
S

[sinha_nsit]

Originally Posted by Toddjones ... ... G32 Z-4. E.8 G0 X1.05 Z-2.0444 X1.3 G32 Z-4. E.8 G0 X1.05 Z-2.0444 X1.3 G32 Z-4. E.8 ... ... My machine does not recognise G32 ...

Use F for lead in the G32 block. At least in Fanuc F is used.

[stxmuddawg]

Originally Posted by Toddjones Hi all, I'm very new to CNC and have plunged into it head first. A friend of mine is a CNC machinist however is experiance is limited in lathe work as it relates to the G Codes. We tried to perform a simple ID threading operation but I either get an Alarm or it does something weird. Here is the code! % O0800 G20 (PROGRAM NAME - XXXXX DATE=DD-MM-YY - 16-09-04 TIME=HH:MM - 17:10 ) (TOOL - 1 OFFSET - 1) (ID THREAD - MIN. .5 DIA. INSERT - NONE) G0 T0101 G97 S200 M03 G0 G54 X1.05 Z-2.0358 M8 X1.2688 G99 G32 Z-4. E.8 G0 X1.05 Z-2.0403 X1.2852 G32 Z-4. E.8 G0 X1.05 Z-2.0444 X1.3 G32 Z-4. E.8 G0 X1.05 Z-2.0444 X1.3 G32 Z-4. E.8 G0 X1.05 Z-2.0358 M9 G28 U0. W0. M05 T0100 M30 % My machine does not recognise G32 and I was advised to switch it to G92. It runs without an alarm using G92 however it does not perform the operation as it is suppost to. It seems to reverse the operation. My machinist said if I try running it I will crash the machine. I am very frustrated as I need to make parts with an ID threat. Any suggestions would be appreciated. He advised that there are no proper Post processors for HAAS lathe's and that I believe the said the closest POST processor is MFLAN. Thanks Todd! PS I hope I posted this in the right area!

what thread are you trying to cut?

[stxmuddawg]

G76P020060Q20R.001
G76X(MINOR OR MAJOR DIA.)Z(DEPTH)R(TAPER IF ANY)P(THREAD HEIGHT)Q(DEPTH OF CUT)F(PITCH OR FEED)

FOR A 1/2-20 ID THREAD

LIKE THIS: G76P020060Q20R.001
G76X.5Z-.5R0P250Q20F.05

THE (R.001) IS HOW MUCH STOCK THE SPRING PASS REMOVES

THE (G76P02) THE 2 IS HOW MANY SPRING PASSES IT MAKES.

G76P020060 THE (60) ON THE END MEANS 60 DEGREE TOOL.

THE (P) IN THE SECOND LINE IS THREAD HEIGHT PER SIDE:SO (P) WOULD BE .025 OF AN INCH, BUT YOU CANNOT USE DECIMALS FOR THE (P)

[g-codeguy]

It always helps if you give the control being used at the very least. Machine you are using helps too. As already stated, F is used on Fanuc controls for threading. At least on the ones I am familiar with. We had some Hardinge CHNCs that used E, but can't recall the control model. If I recall correctly these CHNCs used G33 for threading, not G32. Pretty certain the ones we had when I first start had Allen Bradley controls and used G33.

Are you running a special thread? Must be as .0833 is a 12 pitch thread. You would need at least X1.312 for a 1-5/16 thread. Several thousandths more if using a generic insert instead of a topping one of the correct pitch for the thread being made.

G92 is not complicated to use. Easier than the G32 you are currently using. I prefer the G76 cycle so I can control compound infeed easier.

If I remember correctly, here is how a G92 is programmed:

G0 G54 X1.05 Z-2.0358 M8
G92X1.2688Z-4. F.0833
X1.2852
X1.3
G0G28U0W0M5
M30

Are you truly trying to thread that course of a thread in 3 passes? Not normally advisable. However I did ONE time make a 5/16 inch thread (course, but don't remember the pitch) with 3 passes in softer material as that was the only way I could eliminate chatter.