G81 Drilling

I need to drill a large number of holes,
i've posted all my X & Y values, and added the required G81. However, even though I've followed the Dialog rules for the G81 format, I am still thinking along the lines of Fanuc.

Example,

this is something like what I've done

G17 T1
S+1000
G0 X100 Y100
G0 Z2
G81 (BLAH BLAH BLAH)
G0 X110 Y100
G0 X120 Y100
G0 X130 Y100
,,,
AND SO ON

WITH FANUC, THE MACHINE WILL DRILL AFTER EACH 'G0' COMMAND, BUT THE DIALOG JUST MOVES TO THE NEXT POSITION.
HOW DO I COMMAND IT TO REPEAT THE DRILL CYCLE AFTER EACH 'G0' MOVE ?

Rider-83

The drill cycles are not modal so you will have to do something like the following;

First, in your parameter table, load all of the cycles that you would like to use in each hole position, for example;

P1=G81TA-2.5 (SPOT DRILL CYCLE)
P2=G83TA-38.1MI3HI.3 (PECK DRILL CYCLE, 38.1 MM DP, 3 MM PECK WITH FULL RETRACT BETWEEN PECKS AND .3 MM CLEARANCE )
P3=G84TA-25.4ST1.5875 (TAP CYCLE, 25.4 MM DP WITH 1.5875 PITCH)

Then format your program as follows

N10 G17T1M6
N20 S1000F50M3M8
N30 G0*1X1Y1Z2;P1 (GO TO POSITION AND CALL DRILL CYCLE)
N40 X10Y10;P1
N50 X20Y20;P1
N60 PP1 (Global parameter call, PP1=G0Z200TOM9)
N70 G17T2M6
N80 S750F50M3M8
N90 P1=P2
N100 L1N30N50
N110 PP1
N120 G17T3M6
N130 S250M3
N140 P1=P3
N150 L1N30N50
N160 PP1
N170 M30

Writing your programs using parameters P*, global parameters PP* and looping the program makes for very short code. It is different than Fanuc but is very quick to program and powerful if you take advantage of the functionality. I have done a lot of this including math functions and logic statements so if you have any questions I may be able to help.

Glenn @ Metro North.

Rider:
Can also run this with sub routiens:

N1 G0 X0 Y0 Z100
N2 G17 T1
N3 GO x100 Y100 Z2 N*1
N4 G0 x110 Y110 N*1
N5 G0 X120 Y100 N*1
N6 G0 X130 Y100 N*1
....
.... Continue for all required drilling locations.....
....
N98 G0 Z100
N99 G17 T2
N100 L1 N3 N98 N*2 (call for repeat of all program lines from number 3 to 98 but run sub routien #2 )
N 101 G0 X0 Y0 M30

N*1 G81 F .5 S+1000 Z-7.5 G4F .5 (center drill)

N*2 G82 F .6 S+ 500 Z-20.5 Z-6.0 Z.25 G4F.5 (peck drill through or what ever)

Nice thing about this is each cycle is complete and you can taylor each to give the best results.

To enter a sub simply press the (X as in times, not the axis description) when you are in mode 11 and enter the local sub as any normal program line. To return to the main program hit the "X" key again.
Cheers Ross

Thank you Gentlemen,
I shall study both methods. Ross, your method is what I need. But I'm fascinated with the parameter method, and shall look into this much further. What amazes me about the Dialog control is how advanced it was for its day, even by todays standards

Glenn:
I am a bit confused with some of your sample code.
First off i believe that we are talking Dialog4 here. (think that is what Rider has).
Not seen a D4 control programmed with an M6 or an M3 before. Can you explain how this works. (Thought that a spindle on and direction was simply an "S" plus or minus code for the direction, along with a value for the RPM.
Is the machine you are programming an "AT" and so the use of the M6?
Can you explain how to enter the "PP" in a program line. I have used the peramiter programming some but all local routines with the defined values stored in register #12. On my D4 i can't enter a "PP" the control won't allow it. What is the trick? Where is the "PP" information stored?
Cheers Ross

AlfaGTA;

The code that I wrote was applicable to a Dialog 11 machine. I'm not sure how much of it was compatible with the D4. If you want to try, the parameters (P_) and global parameters (PP-) are under a subdirectory of the programming mode. On the machines I ran they were soft key selections at the same menu level as the programs. The nice thing about them was that you could also call subroutines from a parameter. In the example that I wrote, you could have had a chamfering subroutine (%*_) written in incremental code and simply called it up with a parameter and looped the same program again.

But...., This all could be nothing but a waste of your time if the D4 doesn't use them. It's fun thinking about it though.

Glenn @ Metro North.

Glen:
Thanks for the reply, Dialog11 is different form the D4. Don't think the Dialog4 has the global peramiters. The local peramiters (P) work as you indicate however. Thanks for the information.
This also explains the use of M3, and M6 instructions in your code.
Cheers Ross