[firekoe]

i have a program like this
T1111
G97 M3 S1200
G0 XO. Z.1
G83 Z-1. Q.05 R.1 F.005
G80
G28 U0. W0.
T1100
i am using a fanuc oi-TC and it comes up with a alarm that there is an illegal decimal point. all i am trying to do is drill a hole in some stock with the drill with NO live tooling can some one help

[christinandavid]

Can't see any obvoius problem, are you sure the problem does not lie further on in the program, your control may be looking ahead a lot further than you think...

DP

[firekoe]

there is nothing else to the program

[dcoupar]

Can't have a decimal in the Q. Try Q500

[firekoe]

what is Q500 = to ?

[Karl_T]

what is Q500 = to ?

The number of tenths in the peck, or 50 thou, or 0.05"

Karl

[Superman]

i have a program like this
T1111
G97 M3 S1200
G0 XO. Z.1 <---- try a zero instead
G83 Z-1. Q.05 R.1 F.005
G80
G28 U0. W0.
T1100
illegal decimal point.

O address dosen't have a decimal

come on guys.... this is basic,,, don't try to guess his problem, read all the code first, if he doesn't actually say on which line his program alarmed

[sinha_nsit]

Yes, replace O with 0. Q has to be in mm or inch (your program is ok).

You are not using live tooling, or it is not available on your machine?
The drilling canned cycles are meant to be used with live tooling. So, if live tooling is not available, there is a possibility that these canned cycles are not enabled on your machine. This is what somebody commented in one of the threads.

For drilling at the center, G74 also can be used, if G83 etc. is not available. In G74, Q has to be in steps of 0.0001 inch (or in microns in millimeter mode).

[firekoe]

the program on the machine has the X.0 not X.O just a typo sorry for the confusion. The machine does have live tooling but i am just trying to drill with the drill mounted in a callit in a boring bar pot and i just need to drill a one inch deep hole in a work piece. I don't want to program a peck cycle line by line and i don't have the z axis live tooling pot in the territ so how would i do this. (would it just be ezer to just mount the z axis live tooling pot)

[s&swelding]

I COPIED THIS OUT OF A WORKING PROGRAM THAT I RUN ON MY LATHE W/ FANUC 0i-TC
HOPE THIS HELPS

(TAP DRILL)
(11/32" TWIST DRILL)
G18G54G99
T0808
G50S3000
G97S556M3
G0X0.0Z0.1M8
G83Z-.6R0.Q7000F0.006
G80
G97S400
G0G28U0.W0.M9
M1

Q7000 IS = TO .7 / INCH PECK INCREMENT. BASICALLY THERE IS NO PECK IN THIS CYCLE BECAUSE THE PECK IS EQUAL TO THE START PLANE PLUS THE DEPTH.

[firekoe]

what is the G18 and G54 do?

You don't need the G0 before the G28 U0. W0. as a G28 references return in the oi-TC series control atomically does it under raped traverse

[Sea_en_see]

G18 is the xz plane selection. G54 is the work offset.

[firekoe]

that clears things up. Isnt the machine defaulted to the xz plane from start up?

I have never had to use this code. I don't use the G54 as i set my work offset in a different manner where i don't have to call a G54. The only places i use this is in the milling machines and just wanted to make sure that it was the same thing for the lathes.

Thanks for the clarification

[sinha_nsit]

Is Q-value in mm or microns (in G21)? The manuals have confused me.

0i MB Operators' Manual on page 149 has given example:
G90 G99 G83 X300. Y-250. Z-150. R-100. Q15. F120;
which indicates that it is in mm.

On the other hand, 0i TC Operators' Manual on page 164 gives example:
G83 Z-40.0 R-5.0 Q5000 F5.0 M31;
where M31 is for C-axis clamp. Here, Q is in microns.

This means that on lathe, Q is in microns, but it is in mm on a milling machine. Is my interpretation correct?

[gabedrummin]

Duper.....The dog is correct ....I have a Oi-TC it dose not like a decimal point on the Q .......NOW Way..........