G32 tapping problems

hi i was looking some advice on G32 tapping, when we program the machine to tap the hole like

G28 U0 V0 W0
G97 S320 M03
M08
G99
G00 X0 Y0 Z5.00
G32 F1.25 Z-25.00 M05
G04 X.5
G32 Z5.00 M04
G28 U0 V0 W0
M30

The problem happens at M04, when we reverse the chuck to pull out off the hole, the chuck spins two or three times until its up to rpm then the z axis moves, were using a tapping head with float and clutch the size is m8 x 1.25, is there something im missing ive got a work around with g01 and m codes to shut off the override but its a pain

any help would be great

cheers paul

IeliteENGINEER said:

hi i was looking some advice on G32 tapping, when we program the machine to tap the hole like

G28 U0 V0 W0
G97 S320 M03
M08
G99
G00 X0 Y0 Z5.00
G32 F1.25 Z-25.00 M05
G04 X.5
G32 Z5.00 M04
G28 U0 V0 W0
M30

The problem happens at M04, when we reverse the chuck to pull out off the hole, the chuck spins two or three times until its up to rpm then the z axis moves, were using a tapping head with float and clutch the size is m8 x 1.25, is there something im missing ive got a work around with g01 and m codes to shut off the override but its a pain

any help would be great

cheers paul

Click to expand...

Hi Paul,
Knowing the control make and model will be a help, but its probably a parameter issue, as G32 is normally the same as G01 but with the Feed Override shut out. If you're otherwise happy with the G01 workaround, and your control has a User Macro Option, you could write a Custom Tapping Macro as follows. This example is for a Fanuc control, but will work for many other makes of controls, or can be rewritten in the required format.

Register the number 84 to create a Custom Macro Call with G84, then call the Macro Program with the following Block:

G84 Z-25.000 R5.000 F1.25

O9010
IF [[#9 EQ #0] OR [#18 EQ #0] OR [#26 EQ #0]] GOTO100 (Error Trap for missing required data)
#3004=3 (Disable Feed Hold and Feed Override)
G01 Z#26 F#9 M05
G04 X.5
G01 Z#18 M04
#3004=0 (Enable Feed Hold and Feed Override)
GOTO900 (Finished and no errors)
N100 #3000=1 (MISSING REQUIRED DATA)
N900
M99
%

Regards,

Bill

angelw said:

Hi Paul,
Knowing the control make and model will be a help, but its probably a parameter issue, as G32 is normally the same as G01 but with the Feed Override shut out. If you're otherwise happy with the G01 workaround, and your control has a User Macro Option, you could write a Custom Tapping Macro as follows. This example is for a Fanuc control, but will work for many other makes of controls, or can be rewritten in the required format.

Register the number 84 to create a Custom Macro Call with G84, then call the Macro Program with the following Block:

G84 Z-25.000 R5.000 F1.25

O9010
IF [[#9 EQ #0] OR [#18 EQ #0] OR [#26 EQ #0]] GOTO100 (Error Trap for missing required data)
#3004=3 (Disable Feed Hold and Feed Override)
G01 Z#26 F#9 M05
G04 X.5
G01 Z#18 M04
#3004=0 (Enable Feed Hold and Feed Override)
GOTO900 (Finished and no errors)
N100 #3000=1 (MISSING REQUIRED DATA)
N900
M99
%

Regards,

Bill

Click to expand...

How do I register g84 as a new code? The work around OK but it not great

IeliteENGINEER said:

How do I register g84 as a new code? The work around OK but it not great

Click to expand...

Hi Paul,
You need to specify the Make and Model of the control to get advice on how to create a Custom Macro "G" code.

Of course everyone has their own opinion as to the worth of a solution. I understand that your original issue is with the use of G32 in a tapping situation, but even if you didn't have such an issue with G32, specifying G84 Z_ _ R_ _ F_ _ would be, in my opinion, be a better solution than having to regurgitate the following each time a tapping process needed to be made. The Custom Macro specified in my last Post takes care of Feed Rate Override that you're concerned with when using G01 instead of G32.

G32 F_ _ Z_ _ M05
G04 X.5
G32 Z_ _ M04

In the case of no issue with G32, the Tapping Custom Macro would be as follows.

O9010
IF [[#9 EQ #0] OR [#18 EQ #0] OR [#26 EQ #0]] GOTO100 (Error Trap for missing required data)
G32 Z#26 F#9 M05
G04 X.5
G32 Z#18 M04
GOTO900 (Finished and no errors)
N100 #3000=1 (MISSING REQUIRED DATA)
N900
M99
%

Your machine has a "Y" axis and therefore, presumably a "C" axis and Live Tooling. Most machines of this construction have tapping cycles G84/G87 etc. This being the case, you could live tool tap at the X centre line, but using a revolving workpiece when tapping on centre will give the better result. If it is a case where the control has a G84 Live Tool tapping cycle, you will have to use a different Custom "G" code; perhaps G184.

Post back the Make and Model of the control, and I, or one of the Forum members will advise you on how to create a Custom Macro "G" code. It's a simple procedure irrespective of the control, but the exact process is control specific.

Regards,

Bill