Need Help!- Peck drilling on a 16/18i?

[TheMoose]

I am wondering if it's possible to write a macro of sorts for more efficient peck drilling on a Fanuc pro 3 controller 16i I believe. The control defines all of it z steps (pecks) as one value of Q. I am used to a peck drill cycle defined with I,J and K values. Any way to make this happen? Thanks for your time and attention.

[Metalcutter]

If you have the Macro B option then I would say yes you can probably write a fairly simple yet flexible variable peck drilling routine to increase efficiency. Otherwise it would have to be all linear Z moves and will be a very lengthy program. If you have several holes though, it could be run as a sub program.

[stevo1]

What do you mean more efficient peck drilling cycle??? Do you mean that you are just use to using I,J,K for a pick size and do not want to use the Q value?

I have macros that I wrote for single holes, multiple holes X,Y cord or multiple holes rotary axis. It is possible to set up the pick value in the macro to be variable I,J,orK so when you write your main program it is called I,J,or K and the macro uses the Q of your I,J,K value.

Is this what you need for more "efficient" peck drilling or am I missing something? Let me know if you want me to post any of the macros. These macros are very short and easy to understand.

Stevo

[Metalcutter]

I could be wrong but I think he wants to use varied peck depths in one cycle, eg: first peck 3x drill dia, second peck 2x drill dia... etc.
Some controls do this automatically, some have built in provisions, Every fanuc I've ever seen only had one peck increment defined by the Q word.

[g-codeguy]

If Metalcutter is correct in his assumption, then yes you can write a more efficient drilling cycle if the machine has Macro B. Macro B would allow you to use I, J & K for three of the variables.

Using a variable drill depth is definitely faster than having to use the same increment value for every peck.

[TheMoose]

Originally Posted by Metalcutter I could be wrong but I think he wants to use varied peck depths in one cycle, eg: first peck 3x drill dia, second peck 2x drill dia... etc. Some controls do this automatically, some have built in provisions, Every fanuc I've ever seen only had one peck increment defined by the Q word.

Bingo! That is exactly what I am looking for. This macro would be needed for a large amount of holes all at variable depths. Where do I go from here?

[g-codeguy]

Originally Posted by TheMoose Bingo! That is exactly what I am looking for. This macro would be needed for a large amount of holes all at variable depths. Where do I go from here?

Find out if you have Macro B. In MDI type in #100=5 EOB, hit cycle start. Did it alarm or put 5. in #100 macro?

[Will1]

We have a Fanuc 18-t control on our lathe and the control came with a macro called "VARIABLE DEPTH INCREMENT AUTO CYCLE" to give more flexibility over the old G74 peck drill.
It was a manufacture addition. So I am not sure if it is universal with all Fanucs.

In the program it is a standard macro call out of G65.
Here is a sample from a program after the tool call.
Insert this in the program:

G0X0.Z0.05
G65 P9136 K-.430 B.03 F.001 W.05 C.02 A.3
G0Z.5

Variables for reference:

K= FINAL DEPTH
B=START INCREMENT
F=FEEDRATE
W=DEPTH FIRST PECK
C=MINIMUN PECK INCREMENT
A=DWELL (in seconds at retract)

This program #O9136 is stored in the program library.
Save this as its own program:

:9136(DEEP DRILL)
IF[#6GE0]GOTO70
G00W0.
#4=#5002
#3=ABS[#3]
#2=ABS[#2]
IF[#19EQ98]GOTO1
#19=99
N1G#19F#9
#27=ABS[#23]
#28=ABS[#6]-ABS[#26]
#29=ABS[#26]
DO1
IF[#27LE#3]GOTO2
GOTO3
N2#27=#3
N3IF[#27GE#28]GOTO4
G00Z[#2-#29]
G1Z-[#29+#27]
G00Z#4
G4U#1
#28=#28-#27
#29=#29+#27
#27=#27*.5
END1
N4G00Z[#2-#29]
G1Z#6F#9
G00Z#4
M99
N70#3000=1(K MUST BE NEGATIVE)

Hope that this helps.

Will

[g-codeguy]

Will, that is the same program that came with our Hardinges with 18T controls. Before that it was slightly different program, G65P9135K-.8B.02F.005J.2C.15A.5 on the Hardinges with OT controls. Not quite as useful. Hardinge calls them DEEP DRILL CYCLE.

However, none of the Daewoos with 18T or 21i controls had this program. I have an idea it is specific to the machine manufacturer whether or not you get the program.

That is the program I was going to suggest if Moose has Macro B.

[TheMoose]

Originally Posted by g-codeguy Find out if you have Macro B. In MDI type in #100=5 EOB, hit cycle start. Did it alarm or put 5. in #100 macro?

I typed it in and no alarms. I entered the text without any spaces but when I hit EOB and Insert it shows as #100 =5, and when I hit cycle start the code dissapears

[g-codeguy]

Originally Posted by TheMoose I typed it in and no alarms. I entered the text without any spaces but when I hit EOB and Insert it shows as #100 =5, and when I hit cycle start the code dissapears

Sounds like you have Macro B. If you had gone to the Offset page and hit the far right hard key until "MACRO" came up, and then hit the soft key under Macro, you should have seen 0005.0000 in the 100 macro.

Load the 9136 program Will posted. Give it a shot. In case it isn't clear, B is the incremental distance the drill rapids to from the previous drill depth. So if it is W.5B.02A.2 the first peck will drill to Z-.5, rapid back to the approach location you programmed, dwell .2 second, and rapid to Z-.48 and feed again.

I didn't compare the 9136 Will posted to the one I use, but am going to assume for the time being that it is the same. I can check it out tomorrow to be sure. I mention this because there is a value missing from his G65 call example. You can also define a Z value.

This can be very handy if you are drilling a casting that has a counter bore cast in at say -.5 depth. If you were facing .05 off the face, you would program say Z-.45 (or a little less to be safe) at the end of the G65 call, and it would rapid to Z-.43 (for B.02), and then start feeding. Works the same way if you drill with two different size drills. Drill with the larger one, program Z for that depth in the G65 Macro call, and the smaller drill rapids to the specified clearance point.

I've been using this subprogram for around 20 years with excellent results.

EDIT: BTW, Z0 is understood if there is no Z value in the macro.

[TheMoose]

Thanks for the info thus far! Is there any way for a macro to drill an array of holes all at varying depths? As in not having the macro define the depth of the hole(s) just the pecking depths?

If that makes any sense at all. Here is a sample of what I am doing with I, J and k's in another controller (Fadal) Note the z depths are all different, but the pecking is the same.

N13G83G99X-2.2403Y.6331Z-1.6875R0.1I.85J.6K.15F35.
N15G80
N17G83G99X-3.6688Y-.276Z-1.56R0.1I.85J.6K.15F35.
N19G80
N21G83G99X-1.461Y-.0731Z-.875R0.1I.85J.6K.15F35.
N23G80
N25G83G99X-.5925Y.2679Z-.5625R0.1I.85J.6K.15F35.
N27G80
N29G83G99X-3.1818Y-1.2581Z-2.125R0.1I.85J.6K.15F35.
N31G80
N33G83G99X-2.4269Y-.9334Z-3.8125R0.1I.85J.6K.15F35.
N35G80
N37G83G99X-1.3149Y-.9903Z-2.75R0.1I.85J.6K.15F35.
N39G80
N41G83G99X-.5601Y-1.3393Z-1.4375R0.1I.85J.6K.15F35.
N43G80
N45G83G99X-3.4497Y-1.9075Z-.45R0.1I.85J.6K.15F35.
N47G80
N49G83G99X-1.2581Y-2.2646Z-2.0625R0.1I.85J.6K.15F35.
N51G80
N53G83G99X-2.3214Y-1.7289Z-1.5R0.1I.85J.6K.15F35.