Fanuc G84 rigid tapping code

[Roadstercycle]

Hi, I'm doing some rigid tapping using the fanuc G84 code and was hoping someone could help me out. After tapping a hole it pauses for 3 to 4 seconds before moving to the next hole. Does not seem like a long time but it feels like an hour when your doing production. I just started using the funuc post processor in fusion 360 and hopefully I can fix this. Any help would be appreciated.

Thank you,

Jack

Similar Threads:

• Need Help!- Another Fanuc OM Rigid Tapping Question
• Need Help!- Fanuc 18-M alarm when rigid tapping
• Fanuc OTC rigid tapping help
• Need help with rigid tapping code.

[Jim Dawson]

Can you post a G code snippet, a few lines before and after a G84 cycle.

[Roadstercycle]

Can you post a G code snippet, a few lines before and after a G84 cycle.

Here you go. It's 8 holes tapping.

(DRILL9)
N800 M09
N805 M01
N810 T5 M06
N815 S400 M03
N820 G04 X3
N825 G54
N830 M08
N840 G00 X3.1819 Y-3.1819
N845 G43 Z0.2 H05
N450 M29 S400
N855 G84 X3.1819 Y-3.1819 Z-0.75 R0.2 P0 F20.
N860 X2.7134 Y-2.7134
N865 X1.1092 Y-2.9565
N870 X0.2318 Y-3.0686
N875 X0.3535 Y-0.3535
N880 X0.7866 Y-0.7866
N885 X3.036 Y-1.0296
N890 X3.07 Y-0.25
N895 G80
N900 G00 Z0.2

N910 M09
N915 G28 G91 Z0.
N920 G49
N930 M05
N935 M30
%


Thank you,

Jack

[Jim Dawson]

There is nothing in the G code that would cause the delay. Best guess there is a machine setting that is causing the delay. Something like ''Wait for Spindle Speed Delay'' or something like that. Could be that the spindle is reorienting before continuing on.

[Roadstercycle]

Thank you Jim for taking a look. I did not see anything either but another set of eyes is always a valuable asset. I agree it may be in the machine controller as a delay for all the stars to get aligned before making it's next move.

Jack

[Lomach]

You could try putting a M19 spindle orient before the M29 Line. It might not help but I use it every time.

N840 G00 X3.1819 Y-3.1819
N845 G43 Z0.2 H05
N846 M19
N450 M29 S400
N855 G84 X3.1819 Y-3.1819 Z-0.75 R0.2 P0 F20.
N860 X2.7134 Y-2.7134
N865 X1.1092 Y-2.9565
N870 X0.2318 Y-3.0686
N875 X0.3535 Y-0.3535
N880 X0.7866 Y-0.7866
N885 X3.036 Y-1.0296

[sinha_nsit]

Try G99 G84 instead.

[mikiemus]

Hi,

Dunno about your control but here is a few things to check.

1. the N450, make it to N850.. ( it shouldnt make a difference, if it does.. some of your parameters sux in your control)
2. try to write the whole G84 block for the next hole, as you got in line N855.
3. if you use Fusion360 check out what code comes out of it. Sometimes a M-code (that you run) might mess up things bad.
4. If you use some codes above this snippet of code, be sure they are all set back to 'machine start state'. Like turn on / turn off things.
.... if you turn on something (change it from 'machine power on state') put it back to what it was. (Talking group codes here)

1 question tho. Did the machine do this in the past or not?

I wish you find something useful of all the answers you got from ppl here. =)

Cheers,
Mikie

[generaldisarray]

maybe it all those block numbers. LOL!

have you tried ipr feed? G95
Do not forget to change it back, you'll crap yourself.

[ensign01]

Try removing line N815 you don't need it as spindle speed is defined by the M29 in line N450. This will cause a delay as the spindle is rotating then has to stop and orientate before tapping the hole.

[sinha_nsit]

M03 is unnecessary in rigid tapping.

[m1n1m]

M03 is unnecessary in rigid tapping.

My machine with a Fanuc Mate actually throws a error if I include a speed command (S) with the M03. The Fanuc post processor includes it tho so I have to manually remove it after each post..No idea if that solves anything for you tho ^*

[Roadstercycle]

My machine with a Fanuc Mate actually throws a error if I include a speed command (S) with the M03. The Fanuc post processor includes it tho so I have to manually remove it after each post..No idea if that solves anything for you tho ^*

Thanks everyone for your help, the S400 and M03 above the M29 line was a big factor in the slowness for sure. With the M29 line the M03 is unnecessary. I had been using the S400 with the M03 with no issues or errors.

Jack

[m1n1m]

Let me know if you figure out how to remove this line before a rigid tap cycle. These are modal codes so I assume they have to be reset somehow before a rigid tap cycle. Will poke some at my post processor in a few days and see if I can figure out something.

[Roadstercycle]

Let me know if you figure out how to remove this line before a rigid tap cycle. These are modal codes so I assume they have to be reset somehow before a rigid tap cycle. Will poke some at my post processor in a few days and see if I can figure out something.

I have no idea what your talking about. Why don't you give me the tapping g code example.

[sinha_nsit]

He is probably saying that the spindle is already running.

[m1n1m]

I have no idea what your talking about. Why don't you give me the tapping g code example.

I just assumed that you didn't want to manually edit your gcode after each post containing a rigid tap cycle so you wanted to edit the post processor to leave out M03 SXXX. Also if you had a S commanded earlier in the program it's modal (I think) so it will remain until set to another value. I just tested this the other day on my machine so I'm not very experienced with this.. There's not much of an example to give really. Your code will be good as long as M03 SXXX command is dropped on my machine but this is a bit machine dependent so it's not set in stone what format it needs.

[Roadstercycle]

I manually do my coding. If I do use Fusion 360 then I tweak it. It's no big deal for me because I use the same code a lot. So it is stored.