[colby2000]

Attachment 226078Hello everyone,
I have a part which I'm currently running in a Citizen L20VIII. I attached pic as well as program. Want I want to learn is how to use main tools while part is in sub. I want to deburr milled flats after cutoff using tool 9. I also attached a clip I found on youtube show what I want to do right after cutoff. I'm thinking i can add a k2 argument to my tool call. But I'm not sure where to place it in program so that it follows cutoff;

Thanks Attachment 226078 Attachment 226080


O111255(1-11255 )
$1
(1-112)
M9
G99G97
G18
M6
M52
M87
M97
G113
G50Z.525
G0X.85Z-.05


(.004 TOOL NOSE RAD.)
T0200
M3S1=8000
/B5(HIGH PRESSURE ON)
G0X.8Z0T02
G1X-.02F.002
G0Z-.05
X.6
G1Z.162
X.750,C.01
W.01
G0X.85
Z-.05
X.4
G1Z.162
G0X.85
Z-.05
X.2
G1Z.162
G0X.85
Z-.05
G0X0.
G1Z0F.001
X.185,C.01
Z.164
X.75,C.01
W.01
G0X.85
/B5(HIGH PRESSURE OFF)
G97G0Z-.05T0
M1

G610

(# 2 CENTER DRILL)
T2100
G97M3S1=8000
/B10(HIGH PRESSURE ON)
G99
G0X0.Z-.05T21
G1Z.12F.004
/B10(HIGH PRESSURE OFF)
G97G0Z-.05T0
M1

(2.3 MM NEXUS DRILL)
T2300
G97M3S1=8000
/B10(HIGH PRESSURE ON)
G99
G0X0.Z-.05T23
G1Z.345F.004
/B10(HIGH PRESSURE ON)
G97G0Z-.05G0T0
M1

(M2.5 ROLL TAP)
T2200
G99G18G0X0.
M3S1=2300
/B10(HIGH PRESSURE ON)
G0Z-.05T22
G84Z.340D1F.01772S2300,R1
G80
G0Z-.05
/B10(HIGH PRESSURE OFF)
G97G0T0
M1
M141

G600

M5(STOP SPINDLE)
M18C0
M1

( MILLED FLATS)
T1200(.461 HORN MILL)
T12
G98G19
M59S3=4000
G50W-0.59(LOAD OFFSETS)
/B9(HIGH PRESSURE ON)

(FLAT 1)
G0C0.
G0Y1.35
Z.370
X.61
G1Y-1.07F18
G0X.553
G1Y1.07F12
G0Y1.220
M1

(FLAT 2)
G0C180.
G0X.656
G1Y-.886F18
G0X.496
G1Y1.084
G0X.386
G1Y-1.192
G0X.325
G1Y1.22F12
G0X.275
G1Y-1.192
G0X.900
M1

(FLAT 3)
G0C90.
G0X.582
G1Y.996F18
G0X.472
G1Y-1.104F12
G0X.900
M1

(FLAT 4)
G0C270.
G0X.582
G1Y.996F18
G0X.472
G1Y-1.104F12
G0X.9
Z-.05T0
/B9(HIGH PRESSURE OFF)
M1

(.236 / 6 MM DRILL)
T0800
M58S3=2000
/B9(HIGH PRESSURE ON)
G0C0.
G98G19
G0X.85T08
Z.401
Y-.236
G1X-.6F10
G0X.850T0
/B9(HIGH PRESSURE OFF)
M1

(.375 C-SINK 90/CHAMFER #1)
T0900
M58S3=500
/B9(HIGH PRESSURE ON)
G98G19
G0X.900T09
Z.401
Y-.236
G1X.174F6
G4U0.2
G0X.900T0
/B9(HIGH PRESSURE OFF)
M1

(.157 ENDMILL /.2756 C-BORE# 1)
(ROUGH)
T0700
#510=.265
#511=.1575
#512=.314
#513=6
#514=[[#510-#511]/2]

M58S3=4000
/B8(HIGH PRESSURE ON)
G98G19
G0C0.
G0X.900T07
Z.401
Y-.236
X.5
G1G98X#512F#513
G3W#514K[#514/2]
K-#514
V[#514*2]W-#514K-#514
V-[#514*2]J-[#514/2]

(FINISH)

#500=.2776
#501=.1575
#502=.314
#503=10
#504=[[#500-#501]/2]


G1G98X#502F#503
G3W#504K[#504/2]
K-#504
K-#504
V[#504*2]W-#504K-#504
V-[#504*2]J-[#504/2]
/B8(HIGH PRESSURE OFF)
G0X.9T0
M1




(.375 C-SINK 90 DEG. CHAMFER #2)
(OFFSET # 19)
T0900
M58S3=500
/B9(HIGH PRESSURE ON)
G98G19
G0C180.
G0X.85T19
Z.401
Y.236
G1X.174F6
G4U.2
G0X.850T0
/B9(HIGH PRESSURE OFF)
M1



(.157 ENDMILL/.2756 C-BORE #2)
(OFFSET # 17)
T0700
#510=.265
#511=.1575
#512=.314
#513=6
#514=[[#510-#511]/2]

M58S3=4000
/B8(HIGH PRESSURE ON)
G98G19
G0X.900T17
Z.401
Y.236
X.5
G1G98X#512F#513
G3W#514K[#514/2]
K-#514
V[#514*2]W-#514K-#514
V-[#514*2]J-[#514/2]

(FINISH)

#500=.2776
#501=.1575
#502=.314
#503=10
#504=[[#500-#501]/2]


G1G98X#502F#503
G3W#504K[#504/2]
K-#504
K-#504
V[#504*2]W-#504K-#504
V-[#504*2]J-[#504/2]
/B8(HIGH PRESSURE OFF)
G0X.85T0
M1





(.375C-SINK 90 DEG./.059X45 DEG.)
T0900
M58S3=2000
/B9(HIGH PRESSURE ON)
G98G19
G0X.85T29
G0C-90.
Y-.7
X.450
Z.140
G1Y.7F10
X.38
Y-.7
/B9(HIGH PRESSURE OFF)
G0X.85
G0Z-.05T0
M1

M5(STOP SPINDLE)
M18C0
M1

( MILLED FLATS)
T1200(.461 HORN MILL)
T12
G98G19
M59S3=5000
/B9(HIGH PRESSURE ON)

(FLAT 1)
G0C0.
G0Y1.35
Z.370
X.551
G1Y-1.1F25.0
G0Y1.35
X.9
M1

(FLAT 2)
G0C180.
G1X.275
G1Y-1.28
G0X.900
M1

(FLAT 3)
G0C90.
G1X.472
G1Y1.125
G0X.900
M1

(FLAT 4)
G0C270.
G1X.472
G1Y-1.125
G0X.900
G50W0.59(CANCEL OFFSETS)
G99G40G18M60(CANCELMILL)
G0Z-.05T0
/B9(HIGH PRESSURE OFF)
M1

(ODTURN DEBURR.004 TOOL NOSE RAD.)
T0200
G97M3S1=6000
/B5(HIGH PRESSURE ON)
G0Z-.05
X0T02
G1Z0F.003
X.1572,C.006F.0005
Z.165
X.78
G0X.85
/B5(HIGH PRESSURE OFF)
G97G0Z-.05T0
M1

!L10

( CUTOFF)
N19
T0100
/B4
M87
M97
G97M24M3S1=3000S2=3000
G114.1H1D-2R0.0
G99G18
G0Z1.204
G650(SUPPORT ON)
!L20
!L30
/B4
G50W-0.625(LOAD OFFSETS)
/B1(HIGH PRESSURE ON)
G99
G0X.900Z.579T01
G1X-.02F.003
/B1(HIGH PRESSURE OFF)
G50W0.625(CANCEL OFFSETS)
G97
G113(CANCEL SPIN SYNC)
M86
M96
G600
M5
M25
G4U.5
M8
M8
/M98P8000
M9
M9
M7
G4U.5
G0X-.02Z0.525T0
M6
M56
M53
M118
G999
M118
M5
N999
M2
M99


$2
M118
(SAFE START CODES)
G99
G50Q2000S8000
G50Z0
(END SAFE START CODES)



G610
G600
T3000
G4U.5
G50Z0
M98H21(ABD-125375R)
G50Z0

M98H100(EJECT PART)
!L10

M16(SS OPEN)
M118
G650(SUPPORT ON)
M77(WAIT FOR SYNC)
G0Z-.05
G98G1Z.125F10.0
G4U.5
!L20
G99
M15(SS CLOSE)
!L30
G600
G50Z0

G999
M52
M98H21(ABD-125375 R)
M98H100(EJECT PART)
M53
N999
M2
M99

N21(ABD-125375R)
T3200
G44G97M24S2=6000
G50U0.114(LOAD TOOL OFFSET)
G99G18
/B4
G0Z-.05
X-.700T32
Z0.
G1X0.0F.001
/B4
G50U-0.114(CANCEL TOOL OFFSET)
G97G0Z-.05T0M25
M99

N100(EJECT PART)
M25(SS STOP)
M33
G0Z1.500
M16(SUB OPEN)
M10(KNOCK-OUT ADVANCE)
G4U2.0
/B4
G4U0.5
/B4
M11(KNOCK-OUT RETURN)
T3000
G50Z0
M119
M99



$0
A
#814=0000007500
#815=0000001000
#816=0000001000
#817=0007000000
#822=0000000030
#824=-000000200
#818=0000012820
#819=0000001000
#820=0000000000
#821=0000000520
#990=0000142000
#991=0000051000
#992=0000061000
#893=0000000000
#25119=0000012820
%

[MCImes]

I did something similar. I cut a .008 slot in the part from the sub with the gang tools. Once I had a good part in the sub and my endmill in the main, I moved the Gang into position. Then I recorded Z2 at its home position. I hand wheeled the sub up to the endmill and touched it off until I felt a little drag with a shim. I recorded the Z2 number at the face of the endmill and calculated the difference between the 2. This was my G50Z-6.310 shift in the sub program below.

I cold have done this differently after looking at it again, I didnt need to Z1/Z2 sync, I could have programmed the Z moves in $2 and just had a wait code in $1, but this is how I did it at the time.

So the main thing you need to do is calculate the G50 from Z2 home to the part shimmed to the tool. Once you have that distance, you can program it semi-regularly

Main/$1

IF[#508NE0]GOTO808 (skip mill macro)
IF[#500NE0]GOTO808 (skip mill if sub work disabled)
M5
!2L6 (queue with M98H6 code on sub)
(MILL .008 SLOT ON SUB)
T800
G0Z-.2
G811
!2L800 (sub approach)
M58S3=5000

G1G98X.05F10.T8 (mill slot)
G1X.022F5.
W-.076F1.
X.04F5.
G0W.076

G0X.6M60 (clear)
!2L802
G810 (cancel sync)
!1!2L880
N808




SUB
N6
(CUT .008 SLOT)
T3000
G811 (superimpose)
M118
G50Z-6.310 (calculated from Z2 home to part and tool face)
M48 C0
G0 Z-.1
G1 G98 Z-.008 F10. (arbitrary starting point)
!1L800 (wait for $1 to cut slot)
!1L802 (done cutting slot)

G0Z-.1
G50Z6.310
U0W0T0
G810 (sub home)
G50Z0
!1!2L880 (done)
M99


You probably have it easier if you're only trying to chamfer the back, as it will just be a simple Z move, then Y, with some C indexing possibly.

[danrudolph]

I do this all the time on our A20.

You shouldn't have to worry about that G50 distance that MCImes talked about if you use the K2 argument.

I use two G600's to block around that live tool call in $2. I usually put it after a facing pass on the main spindle, retract the main to Z-.050, then call the live tool with K2 from the sub spindle, do the work, then issue another G600 to let the sub go home.

With K2, the cutoff face of the part is Z0.0 and the centerline of the tool is Z0.0. No G50 like calling the live tools from the main side.

HTH,
Dan

[MCImes]

I do this all the time on our A20.

You shouldn't have to worry about that G50 distance that MCImes talked about if you use the K2 argument.

I use two G600's to block around that live tool call in $2. I usually put it after a facing pass on the main spindle, retract the main to Z-.050, then call the live tool with K2 from the sub spindle, do the work, then issue another G600 to let the sub go home.

With K2, the cutoff face of the part is Z0.0 and the centerline of the tool is Z0.0. No G50 like calling the live tools from the main side.

HTH,
Dan

It might be because Im still using WinCNC 2k, but it doesnt show the K2 argument and I'm not familiar with it. Can you explain or paste the explanation of how this is used? I'd like to use this, as we do this semi frequently. Also, do you know when this became an option/argument?

Thanks

[danrudolph]

From the text file, which I believe is the one from WinCNC:

T0100-T900 *(Front side Gang tools)

T0200 X Y Z Q1 H K2 E

T700 K2

X.3 = Use X to position X after the tool call.

Y.3 = Use Y to position Y after the tool call.

Z.3 = Use Z to position Z after the tool call.

Q1 = Quick index. This will not move to safe position then index,
It will move from where it is to the new tool in a straight line.

H.5 = Temporary change position point for just this one index.

K2 = Used to call the Z2 axis as being programmed. If 'T3100K2' in $1
then X1-Y1-Z2-C2 are programmed in $1. K2 is canceled on any other
Tool call. Also if using 'T100K2' to 'T600K2' the Z2 zero position is
automaticaly set to the back side of the tool knowing the sub spindle
with part face as zero. If 'T700K2' to 'T900K2' is used then the Z2
zero position is automaticaly set to the center of the live tool
knowing the sub spindle with part face as zero.

$1 T0300 $1=X1Y1Z1C1 $2=X2Z2C2
$1 T0300 K2 $1=X1Y1Z2C2 $2=X2Z1C1

$2 T0300 alarm -not alowed
$2 T0300 K2 $1=X2Z1C1 *$2=X1Y1Z2C2


E90.= Use E to save cycle time. The C axis will go to E90. while changing
tools. Do not use M5 and do not use M18

Not sure when this was added and/or to what machines. Like I said, I have this on our A2-20.


Dan

[MCImes]

Thanks for that. That function must have come along after 2005, as thats when our L20's are from and they wont accept the K2 modifier.

Good to know though. Thanks again