Peck Drill on a 21M fanuc control?

ben29 · May 23, 2017

I'm working on a Chiron FZ 12W with a 21M control and I cant get a g83 or g73 to work. I have a lot of small holes I need to peck. Is this control capable of peck tapping? It keeps alarming to an Improper G code.

Thanks, Ben

yardbird · May 23, 2017

Your machine doesn't have the option turned on.

Brent

triumph406 · May 23, 2017

ben29 said:
I'm working on a Chiron FZ 12W with a 21M control and I cant get a g83 or g73 to work. I have a lot of small holes I need to peck. Is this control capable of peck tapping? It keeps alarming to an Improper G code.

Thanks, Ben

Is there a 'Q' value on the same line to specify peck depth?

something like

G83 X0 Y0 Z-1.2 Q.2500 R0.1 F15.0

yardbird · May 23, 2017

triumph406 said:
G83 X0 Y0 Z-1.2 Q2500 R0.1 F15.0

I believe what you have would run. But it's getting hung up on the G-code.

Try to execute a G83 in MDI and see if you get the "improper G code" alarm?

Brent

Booze Daily · May 23, 2017

Need a G98 or G99 so it knows where to retract to between holes?

Vancbiker · May 23, 2017

Improper G code alarm is a sure sign that the control is missing the option for canned cycles. Pretty unusual as most builders, Chiron included, provide the Fanuc option as a standard feature. I'd suggest checking your 9000 range parameter against the original parameter list if available.

ben29 · May 24, 2017

My g83 is something like g83 g98 Z-1. R.1 Q.2 F25. I guesd i'll call them this morning or I can just keep repeating the G81 at different depths which is a pain. Thanks guys

Sent from my SAMSUNG-SM-G891A using Tapatalk

sinha · May 24, 2017

Try Q2000 without decimal.

triumph406 · May 24, 2017

sinha said:
Try Q2000 without decimal.

On a Fanuc 0M (at least mine) if the Q value is Q2000 it ignores the peck value and drills to the full depth without pecking.

sinha · May 24, 2017

It looks unusual to me. Bill may have an explanation.

tay2daizzo8 · May 24, 2017

if u can g81 it then g83 should be no issue..was a previous canned cycle not canceled using g80?

sinha · May 24, 2017

Logically, when a new canned cycle is commanded, the previous one should automatically get canceled.

tay2daizzo8 · May 25, 2017

they dont automatically cancel..especially fanuc..on my robodrill if you reset/alarm in middle of canned cycle or comp it will throw an atc error untill you MDI g53 g40 g80 z0

angelw · May 26, 2017

triumph406 said:
On a Fanuc 0M (at least mine) if the Q value is Q2000 it ignores the peck value and drills to the full depth without pecking.

Hello triumph406,
Fanuc controls can be set via parameter to what they refer to as Pocket Calculator Mode, meaning that values can be specified without a period and assumed to be Integers, rather than the Least Programmable Increment for the control. For example, in Pocket Calculator mode, the following:

X10

will be read as 10.0 rather than 0.010 (metric mode with a Least Programmable Increment of 0.001).

If Pocket Calculator Mode is set on your machine, it would explain why Q2000 seams to be ignored. In Pocket Calculator Mode, Q2000 would represent 2000mm, or 2000" and therefore, greater than the depth of any hole you may be drilling. If the Q value exceeds the full depth of the hole, no alarm is raised and the cycle is performed with no peck.

Regards,

Bill

sinha · May 26, 2017

Bill,
I believe many machines are set for calculator mode because it is safer and logical. How is Q specified on such machines. I am under the impression that Q is independent of this mode, and it is always in least increment.

angelw · May 27, 2017

sinha said:
Bill,
I believe many machines are set for calculator mode because it is safer and logical. How is Q specified on such machines. I am under the impression that Q is independent of this mode, and it is always in least increment.

Hello Sinha,
Calculator mode is not the Fanuc default. Overwhelmingly, they are set to least programmable increment.

On many early machines I've been asked to set to Calculator mode, cycles using addresses where a period in not accepted, its been handled quite badly. On some, neither least programmable increment, nor decimal input worked. On others, they accepted Least Programmable Increments.

Q is an address that accepts a period. Accordingly, if Calculator Mode is selected and the period is omitted, an Integer value will be assumed.

Regards,

Bill

sinha · May 27, 2017

triumph406 said:
On a Fanuc 0M (at least mine) if the Q value is Q2000 it ignores the peck value and drills to the full depth without pecking.

So many things are control/model/parameter dependent that it is difficult to say anything with certainty.
What works on your machine: Q2 or Q2.0 or something else?
What is X10 on your machine: 10 mm or 10 microns (0.01 mm)?
I am wondering if P and Q in the lathe canned cycles G74/G75/G76 have similar issues.

angelw · May 28, 2017

sinha said:
So many things are control/model/parameter dependent that it is difficult to say anything with certainty.
What works on your machine: Q2 or Q2.0 or something else?
What is X10 on your machine: 10 mm or 10 microns (0.01 mm)?
I am wondering if P and Q in the lathe canned cycles G74/G75/G76 have similar issues.

Hello Sinha,
I tried the alternatives on an OM (circa 1998) and an 18i Fanuc control.

With both controls set to Pocket Calculator Mode, with the period omitted, Q express an integer for both controls. That is, Q5 gave a Peck Distance of 5.0mm; Q5.0 gave the same result. With Pocket Calculator Mode turned off on both controls, Q5 gave a Peck Distance of 0.005mm for both controls; Q5.0, as per normal, gave a Peck Distance of 5.0mm.

Regards,

Bill

sinha · May 28, 2017

Bill,

So, there is no difference in the behavior of X and Q in different modes. Did I understand it correctly?

Please also check the effect of mode selection on the lathe canned cycles (P/Q words) on the two controls, whenever you have some spare time.

Thank you so much for the kind of information you give.

angelw · May 28, 2017

sinha said:
Bill,

So, there is no difference in the behavior of X and Q in different modes. Did I understand it correctly?

Please also check the effect of mode selection on the lathe canned cycles (P/Q words) on the two controls, whenever you have some spare time.

Thank you so much for the kind of information you give.

Hello Sinha,
Pocket Calculator Mode has an affect only on addresses that can tolerate a period. Accordingly, the P address has the same value in either mode. Also, the G code that precedes the address has an affect on how its processed.

For example:

G20 (Input in inches)
X1.0 G04
In the above example, because X1.0 preceded G04 in the one block, its considered to be a distance and processed as X10000 by the control. This command is equivalent to G04 X10000. The Least Programmable Increment for seconds is 0.001, therefore, the tool dwells for 10 seconds.

G04 X1.0
In the above example X1.0 is processed as a time period (seconds) and is equivalent to G04 X1000. Therefore, the tool dwells for one second.

Regards,

Bill

Peck Drill on a 21M fanuc control?

Aluminum

Titanium

Diamond

Titanium

Titanium

Diamond

Aluminum

Titanium

Diamond

Titanium

Hot Rolled

Titanium

Hot Rolled

Diamond

Titanium

Diamond

Titanium

Diamond

Titanium

Diamond

Similar threads