program for leblond makino

[MATT Q]

Is anybody using a gf6 leblond makino VMC with the swing arm tool changer? What I was wondering is if anybody has a small program for a machine like this with some tool changes so I can send it to my mastercam dealer for a post to be produced for me. can anybody help me out? Pleaseeee:)

[Brendan P]

Matt,

Have you ever done a tool change with this machine?

We have a fnc74 leblonde makino that has to call a dummy tool first in order for it to recognize

the pot numbers.

Also when calling the M6,the control then calls a

9000 type sub prog. which actually changes the tool.

Not sure if this is the info that you are looking for.

[specv]

We have a FNC106 VMC let me know what info you need.

pete

[Reece L Gibson]

I have Experience with this type of machine.

Had a 6T Fanuc on it.It would not remember what tool was in the spindle when it was shut off.

We rewote the Tool change Macro (program #9000)

set-up a variable to record what tool was in the spindle all the time so it would skip tool changes if the tool was already in the spindle(even when the power was turned off).

[Rekd™]

quote:

---

It would not remember what tool was in the spindle when it was shut off.

We rewote the Tool change Macro (program #9000)

set-up a variable to record what tool was in the spindle all the time so it would skip tool changes if the tool was already in the spindle(even when the power was turned off).

---

It's bad that this issue was not resolved by the manufacturer, (WTH were they thinking?), but it's good that you're able to "patch" it via macros.

 

 

'Rekd

[McRae]

quote:

---

it would skip tool changes if the tool was already in the spindle(even when the power was turned off).

---

What are you doing trying to change tools with the power turned off?

[MATT Q]

This is what I have guys it has a professional 3 fanuc system 6m model B for the controller I guess. Bare with me guys haven't had any experience with a machine of this type. The tool changer is the random pot style tool changer. If one of you guys want to e-mail me a program or something so I can get started and see if it will run the program you send me with out any errors or alarms I would owe you some beers:)

[kyle]

Matt, we have a gf6 and exactly what are you looking for, you can mdi a tool change at the control or am I not seeing what you want, is it just a post problem?

[MATT Q]

No I don't have a post for it and I'm looking for a simple program that has some tool changes in it so I can send the program to the mastercam dealer and they can make the post for me I don't currently have a post at all for it and I don't have enough experience with post editing to figure it out on my own.

[specv]

Here is small sample of how ours is

 

O0001(TL5677)

(06/25/03)

N1 G20G0G17G40G49G80G90

N2 G10 L2 P1 X-27.0115 Y-12.746 Z-23.9807

(.750 DIA 2FL HSS SPOTDRILL)

N3 T1

N4 G0G90G54X7.874Y-3.937S800M3

N5 G43H1Z2.M8

N6 G98G81Z-.35R.2F6.

N7 Y3.937

N8 G80M9

N9 M5

N10 M01

(.6406 DIA 2FL HSS DRILL)

N11 T2M6

N12 G0G90G54X7.874Y-3.937S1431M3

N13 G43H2Z2.M8T1

N14 G98G73Z-3.3125R.2Q.225F8.79

N21 Y3.937

N22 G80M9

N23 M5

N24 G91G28Z0.0

N25 G28Y0.

N26 M6

N27 M30

[MATT Q]

Thanks specv for the program:) I'll give it a shot tomorrow if anybody has any others they would be appreciated. THanks guys

[Brendan P]

Matt,

Here is a sample of our Fanuc 6MB program.

 

%

O1234

(MAKINO SAMPLE)

 

G40G80H00M19

 

N1(TOOL 1 OFFSET 1)

( 2" SHELL MILL )

T99

T1M6

T2

S1500M3

G54G90G0X-4.25Y-2.2499

G43Z.25H1M8

Z.1

G1Z0.F30.

X3.95F15.

G0Y-.75

G1X-3.95

G0Y.75

G1X3.95

G0Y2.2499

G1X-4.25

G0Z.25

G0Z1.M9

G28G91Z0.

H00

G28X0Y0

M19

M01

 

N2(TOOL 2 OFFSET 2)

( 1/2 DRILL )

T2M6

T3

S534M3

G54G90G0X-1.7228Y1.0681

G43Z.1H2

G99G83Z-1.2502R.1Q.2F4.28

X-1.3438Y-1.0165

X-.3446Y.758

X1.3782Y1.1887

X1.9985Y-.9303

X.603Y-1.1887

G80

G0Z1.

G28G91Z0.

H00

G28X0Y0

M19

M01

 

N3(TOOL 3 OFFSET 3)

( 1/2 HSS ENDMILL )

T3M6

T99

S2200M3

G54G90G0X-4.Y-.5

G43Z.25H3M8

Z.1

G1Z-1.F30.

X-3.5F12.

G3X-3.Y0.R.5

G1Y2.

G2X-2.625Y2.375R.375

G1X2.625

G2X3.Y2.R.375

G1Y-2.

G2X2.625Y-2.375R.375

G1X-2.625

G2X-3.Y-2.R.375

G1Y0.

G3X-3.5Y.5R.5

G1X-4.

G0Z.25

G0Z1.M9

G28G91Z0.

H00

G28X0Y0

M19

T99M6

M30

%

 

The T99 is the dummy tool.

It must be in the spindle (especially before powering down the machine).

When you call it up in the beginning,you are telling the machine that this is the tool that is in the spindle.

Or else you get that little annoying red alarm light.

Then it will be able to retrieve a tool out of the carousel.

At the end of our program, we put it back in the spindle.

I am not sure if this will be what you need,but this is the way we have to do it.

Also,as I stated earlier,I believe we have (2) 9000 series tool change subs in the main prog. directory that get called up upon an M6 command.

 

Hope this helps and if this is the case,and you need these subs,I can give them to you.

[MATT Q]

Man you guys are great this forum is a very useful tool I owe you guys some beer thanks alot:)

[Reece L Gibson]

That's what I meant by when you shut the power down, It will not remember what tool is in the spindle.We used the common variable #505 to store the current tool number that's in the spindle. We called Makino and they could not help.

[Marklaw]

On 7/9/2003 at 4:53 AM, specv said:

We have a FNC106 VMC let me know what info you need.

pete

I have a FNC106 and we switched out the memory board and we lost the 9000 series tool changing programs

[specv]

here are the 2 that are in the machine

O9001
M9 
G0G28G80G91Z0M5
G49G40 
M6 
G90M99 

O9111
M57
S1T0 
S2T0 
S3T0 
S4T0 
S5T0 
S6T0 
S7T0 
S8T0 
S9T0 
S10T0
S11T0
S12T0
S13T0
S14T0
S15T0
S16T0
S17T0
S18T0
S19T0
S20T0
S21T0
S22T0
S23T0
S24T0
S25T0
S26T0
S27T0
S28T0
S29T0
S30T0
M57
S2T2 
S3T3 
S4T4 
S5T5 
S6T6 
S7T7 
S8T8 
S9T9 
S10T10 
S11T11 
S12T12 
S13T13 
S14T14 
S15T15 
S16T16 
S17T17 
S18T18 
S19T19 
S20T20 
S21T21 
S22T22 
S23T23 
S24T24 
S25T25 
S26T26 
S27T27 
S28T28 
S29T29 
S30T30 
M30
%

[Marklaw]

3 hours ago, specv said:

here are the 2 that are in the machine

O9001
M9 
G0G28G80G91Z0M5
G49G40 
M6 
G90M99 

O9111
M57
S1T0 
S2T0 
S3T0 
S4T0 
S5T0 
S6T0 
S7T0 
S8T0 
S9T0 
S10T0
S11T0
S12T0
S13T0
S14T0
S15T0
S16T0
S17T0
S18T0
S19T0
S20T0
S21T0
S22T0
S23T0
S24T0
S25T0
S26T0
S27T0
S28T0
S29T0
S30T0
M57
S2T2 
S3T3 
S4T4 
S5T5 
S6T6 
S7T7 
S8T8 
S9T9 
S10T10 
S11T11 
S12T12 
S13T13 
S14T14 
S15T15 
S16T16 
S17T17 
S18T18 
S19T19 
S20T20 
S21T21 
S22T22 
S23T23 
S24T24 
S25T25 
S26T26 
S27T27 
S28T28 
S29T29 
S30T30 
M30
%

Thanks for the help.  Do you know how to enable it so I can edit type a 9000 program in?