Rigid & Peck tap

[seattlewa98]

I have been reading about rigid and peck tap thru this and getting

All I want is tapping 1/2 deep, back out tap 1/2 deep more, back out to clearance height ,spindle stop, move on next point and tapping samething again.

Below is what I got

 

1st post

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.S2000M3

N14G43H1Z.1

N15M29S2000

N16G99G84Z-1.R.1Q.5F100.

N17X-.5Y-.25

N18G80

N19M5

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

%

I does exactly what I want but when get to line N17, the machine DOES NOT do anything and spindle still on. What did I do wrong here ?

 

2nd post

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.S2000M3

N14G43H1Z.1

N15M29S2000

N16G99G84Z-1.R.1F100.

N17X-.5Y-.25

N18G80

N19M5

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

%

 

I didn't put Q value in, machine tap all the way down, and DOES NOT do anything at line N17G80

 

3rd post

 

N10 G0 G17 G40 G49 G80 G90

N11 T1 M6 ( )

N12 G0 G90 G54 X-2. Y1. S2000 M3

N13 G43 H1 Z.1

N14 G99 G84 X-2. Y1. Z-.5 R.1 J1 F100.

N15 G99 G84 X-2. Y1. Z-1. R.1 J1 F100.

N16 G99 G84 X-.5 Y-.25 Z-.5 R.1 J1 F100.

N17 G99 G84 X-.5 Y-.25 Z-1. R.1 J1 F100.

N18 G80

N19 M5

N20 G0 G28 G91 Z0

N21 G0 G90 G28 X0. Y0.

N22 G54

N23 M30

%

Does what I want except the spindle DOES NOT stop after back out at clearance height to move on to next hole to tap.

 

To me,

1) M29Sxxxx, and Q value: machine does what I want (peck tapping and spindle stop at clearance height) but does NOT do anything after finish tapping(suppose move to home and end of program)

2) M29Sxxxx, NO Q value: machine is tapping all the way, but wont do anything else after finish tapping

3) NO M29Sxxxx, spindle won't stop at clearance height before move on to next hole location.

[Rick Henrickson 65]

the m29 s is to set up the rigid tap cycle I am guessing this is a fanuc control?

it should just go to the next hole, do you have it in single block? is the control still lit like its running?

[iowajim62]

Try changing these lines in bold and see if it runs on thru to next hole location. All Fanuc Controls are not the same. This may work and may not. I genrally never tap with G99 only G98. Parameter 5200 is where info for Rigid Tapping cycle will be found, consult your machine manual you may have overlooked something.

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.S2000M3

N14G43H1Z.1

N15M29S2000

N16G99G84Z-1.R.1Q.5F100.

N17X-.5Y-.25

N18G80

N19M5

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.

N14G43H1Z.1

N15M29S2000

N16G98G84Z-1.R.1Q.5F100.

N17X-.5Y-.25

N18G80

N19M5

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

[Santa Fe]

At this point, best you can do is refer to your fanuc programmin manual that comes with the machine and follow exactly line by line what it says for rigid tapping cycle. May be you need a G84.1 or to combine G80 with something else in the same line.

[seattlewa98]

Sorry for confused all you guys

 

The machine has Fanuc control

 

1st post

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.S2000M3

N14G43H1Z.1

N15M29S2000

N16G99G84Z-1.R.1Q.5F100.

N17X-.5Y-.25

N18G80

N19M5

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

%

I does exactly what I want but when get to line N18 (not N17), the machine DOES NOT do anything and spindle still on. What did I do wrong here ?

 

2nd post

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.S2000M3

N14G43H1Z.1

N15M29S2000

N16G99G84Z-1.R.1F100.

N17X-.5Y-.25

N18G80

N19M5

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

%

 

I didn't put Q value in, machine tap all the way down, and DOES NOT do anything at line N18G80 (not N17)

 

3rd post

 

N10 G0 G17 G40 G49 G80 G90

N11 T1 M6 ( )

N12 G0 G90 G54 X-2. Y1. S2000 M3

N13 G43 H1 Z.1

N14 G99 G84 X-2. Y1. Z-.5 R.1 J1 F100.

N15 G99 G84 X-2. Y1. Z-1. R.1 J1 F100.

N16 G99 G84 X-.5 Y-.25 Z-.5 R.1 J1 F100.

N17 G99 G84 X-.5 Y-.25 Z-1. R.1 J1 F100.

N18 G80

N19 M5

N20 G0 G28 G91 Z0

N21 G0 G90 G28 X0. Y0.

N22 G54

N23 M30

%

Does what I want except the spindle DOES NOT stop between moving from 1st hole to 2nd hole

[seattlewa98]

According to manual book, M29 and G84 for rigid tap and M29 should be at begining of tapping operation, Is there any M code at the end of tapping operation ?

[Guest CNC Apps Guy 1]

What machine is it?

 

Some machines require an M-Code after the G80 to cancel rigid tapping. Consult your machine's programming manual to see if yours does.

 

From what I'm looking at, your code looks fine and should work. Parameter 5200 determines that type of peck, high speed style or G81 style.

 

I set my cycles to look like the following though,

 

N11G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

N12T1M6

N13G0G90G54X-2.Y1.A0.(NO SPINDLE ON NEEDED HERE)

N14G43H1Z.1

N15M19 (ORIENT SPINDLE IN CASE I NEED TO CHASE THE SAME HOLE)

N16M29S2000

N17G99G84Z-1.R.1Q.5F100.

N18X-.5Y-.25

N19G80

N20G91G28Z0.

N21G90G28X0Y0A0

N22M30

%

 

HTH

[romer]

If you haven't already found this in a search, this may help.

 

http://www.eMastercam.com/ubb/ultimatebb.p...ic;f=1;t=024036

 

Always keep in mind that although different machine builders may use the same Fanuc control, that in NO WAY insures that it will digest the same canned cycles, M-codes, etc. as any other machine with the same control.

 

Always read and refer to the manufacturer's manuals as a place to start.

 

Romer

[seattlewa98]

Problem solved

I went to parameter 5200 and change SIG to 1 for G80 activated