Reply with QuoteHey,
For milling centers with FUNUC controls, I always used G83 or G73 Zyour depth R your distance above + or below- your work Q is your peck amount and F is your feed.I never seen IJK before with FUNUC.
Hope this helps,
KROW
Canned Drilling Cycle Help
I am trying to program a drill cycle to use IJK. I tried G73 and G83 and no luck. "I" being the first peck, "j" being target depth, "K" being subsequent pecks. Does anyone know how to imput this in the FANUC control? Example?
This is what I did, G83G98X...Y...Z...R...I...J...K...F...
Similar Threads:
Hey,
For milling centers with FUNUC controls, I always used G83 or G73 Zyour depth R your distance above + or below- your work Q is your peck amount and F is your feed.I never seen IJK before with FUNUC.
Hope this helps,
KROW
I want my first peck to be .75", then subsuquent pecks to be .10". How do I lay that out?
Hi
For a single hole you could use a G81 for the first 0.75 depth and then the peck drill 0.1 with the G83. You also need to know the finished depth to get the right z value.
This is just for a single hole at 0,0. Do you want to lay out a pattern around an arc or circle with the I and J?
(code macro: drill.point.depth)
G81 F15. R0.25 X0. Y0. Z-0.75
G83 F15. Q0.1 R0.2 X0. Y0. Z-1.5
www.cncprogramdeveloper.com
I have 300 holes. I have c'bore that is .75" deep. I want my R to be .25 above that. I dont want to start pecking 1" above. So I want my first peck to .75". I have used IJK in the past on my canned cycle to make this work, I just cant remember what I did.
On a "Haas" control for peck drilling with G83 the IJK are:
I Size of first cutting depth
J Amount to reduce cutting depth each pass
K Minimum depth of cut
You would end up with something like this.
G83 F15. I0.75 J0.1 K0.1 R-0.5 X0. Y0. Z-1.5
G73 is similar on the Haas.
The Fanuc manual I am reading doesn't have those IJK options.
Hi chuppe
Try this G90G0X0.Y0.
G43Z.1H1
G73G98X0.Y0.Z-1.175R-.700Q.1F12
Z-1.175 Depth you want to go in the part
R-700 Depth were you want to start cutting
The G98 Returns the Z to .1 above the part
The Q.1 Is your Peck
Mactec54
You didn't mention what control you have.... but ...
FANUC doesn't use IJK on its own account. I take that back... some models can use an I and a K but not in the way you're thinking. To do what your looking to do, you can use G73 like Mactec posted. But if you want a full retract after intial peck, you'll need to write the code in long hand and use a macro loop or sub call...
It's just a part..... cutter still goes round and round....
canned cycle G83
Dear Frd , it is not possible with G83 . you have to write your own MACRO cycle for that using I,J & k.
Hole MakingOriginally Posted by chuppe
you need to understand G98/G99 and how these work with the drill cycles, where your tool is positioned before starting the command
G81 ( spot hole )( feed in, rapid out )
eg G81 X,Y,Z,P,R,F,G98/G99
X and Y = hole co-ordinates
Z = final hole depth
P = dwell time at Z depth
R = start point for cycle, retract point after getting to Z
F = feedrate going to Z
G98 = return to Z plane before starting next block/line
G99 = return to R plane before starting next block/line
program example
G0 X0 Y0
G43Z2.H1 ( 2" above Z0 )
G81 Z-1. R-0.1 P.3 F12. G98 ( tool goes to Z-0.1,feeds to 1" deep @ 12" per minute, dwells 0.3 seconds, retracts to Z2 )
but if you alter G98 to G99
G81 Z-1. R-0.1 P.3 F12. G99 ( tool goes to Z-0.1,feeds to 1" deep @ 12" per minute, dwells 0.3 seconds, retracts to Z-0.1 ) ( this is dangerous, if material exists at Z0 and you do more holes )
now the others
G73 ( High speed drilling canned cycle )( feed in, chip break pattern to Z depth, rapid out )
eg G73 X,Y,Z,Q,P,R,F,G98/G99
Q = peck distance
G83 ( Peck drilling cycle )( feed in Q distance, rapid out, back to last point, peck Q pattern to Z depth, rapid out )
eg G83 X,Y,Z,P,Q,R,F,G98/G99
or with Q modified to I & J
G83 ( Peck drilling cycle )( feed in I distance peck to J distance, rapid out, back to last point, peck I distance to J distance type pattern to Z depth, rapid out )
eg G83 X,Y,Z,P,I,J,R,F,G98/G99
I = short pecks to incremental J distance
J = rapid back to R
K = used on lathe
program example
G0 X0 Y0
G43Z2.H1
G83 Z-1. I.05 J.2 R.1 G98 (tool will rapid to Z0.1, peck in 0.05" steps for 0.2", retract to R, rapid to last point, peck in 0.05" for 0.2" ,this pattern till Z-1., then retract to Z2.)
the machine will pause at these points
Z0.10
Z0.05
Z0.00
Z-0.05
Z-0.10
Z0.10 ( retract )
Z-0.10
Z-0.15
Z-0.20
Z-0.25
Z-0.30 ( retract )
..
Z-1.00 ( retract to plane G98/G99) ( and end cycle )
For you to do many holes and to cut time to a minimum ( you can alter values as they are modal also )
G0 X0 Y0
S1000 M3
G43Z.5.H1
M8
G83 Z-1.5 R-.65 I0.1 J0.75 F12. G98
X Y P.1
X Y Z-1.25 P0. R.1
X Y Z-1.5 R-.65
and so on
G80 or G0 ( to cancel canned cycle )( G80, on some machines, stops the spindle )
The IJK I have used in the past was on a HAAS control. The FANUC does not use them the same way. Thanks everyone for your help. I think I will write a quick macro to do what I want.
FANUC dual mode control
am trying to program a drill cycle to use IJK. I tried G73 and G83 and no luck. "I" being the first peck, "j" being target depth, "K" being subsequent pecks. Does anyone know how to imput this in the FANUC control? Example?
This is what I did, G83G98X...Y...Z...R...I...J...K...F...
I worked in a shop with a 4020 and attended the training course that came in the sale to our company. This was in '96 or '97, and then FANUC Controllers could be programmed with the FANUC G-Code configuration, or in Universal G-Code config.
Just a wild thought...does this sound in any way familiar from what you know about your machine/Controller?
next time
next time buy a mazak. i just wrote 20 programs for my 6800 and your still
playing with one program. i never ran a hass but i,j,and k are centerline of arcs!
i think maybe your job plan is wrong. i would have drilled the hole from the top. then counterbore your holes. use a reamer and a spot tool to deburr the hole.
er....dead thread ---- 3 1/2 years old
he's prolly done a 1000 programs by now
Hey Steve!!
Great drill cycle list though.
Thanks, even if thread was a bit old. A great find.
Must meet you one day, being local.
Super X3. 3600rpm. Sheridan 6"x24" Lathe + more. THREE ways to fix things: The RIGHT way, the OTHER way, and maybe YOUR way, which is possibly a FASTER WRONG WAY!
Posting Permissions
