G49

[shredder]

Good morning everyone:)

I need some help with a MyCenter-4xiF_Fanuc30iB  post .

I need to get rid of the g49 on line 3360.Any help greatly appreciated:)

cheers,

 

 

 

 

N3310 (3D S.FINISH)
N3320 (TOOLPATH - FINISHPARL)
N3330 (STOCK LEFT ON DRIVE SURFS = .005)
N3340 (STOCK LEFT ON CHECK SURFS = .005)
N3350 X-.2 Y.0798
N3360 G49
N3370 G05.1 Q1 R1
N3380 G43 H23 Z7.
N3390 Z1.9595
N3400 G01 Z1.7095
N3410 X-.1965 Z1.712
N3420 X-.1709 Z1.7262
N3430 X-.1636 Z1.7302
N3440 X-.1348 Z1.7426

[Guest]

Actually, that should be there

 

The G49 needs to be active before that G05.1Q1R1 call

 

If that's a null toolchange, you may need to setup force toolchange to pick everything up properly

 

You may want to read this

 

http://www.mtbtech.net/blog/2012/11/09/FANUC-AI-High-Speed-Modes-Simplified.aspx

 

 

1. Make sure G49 is called before the execution of G05.1 Q1 Rx

2. G05.1 Q1 Rx must be engaged BEFORE G43-Tool Length Comp

3. AICC and AIAPC need to be turned on and off for each tool

4. AICC and AIAPC does not apply to canned drilling cycles

[shredder]

Thanks

JParis

The problem is I am trying to use this post for a fanuc series oi and it crashes as soon as it reads g49.

[Guest]

Send it home then

 

The issue is the process you're using

 

As I said, if that is a null tool change, use the "Force Tool Change" That will get the G49 out at a point that won't cause an issue

 

That G05 should not be issued the way you're trying to do it

 

 

G00 G91 G28 Z0.

G49

T23 M6

N3310 (3D S.FINISH)

N3320 (TOOLPATH - FINISHPARL)
N3330 (STOCK LEFT ON DRIVE SURFS = .005)
N3340 (STOCK LEFT ON CHECK SURFS = .005)
N3350 G00 G90 G54 X-.2 Y.0798
N3360 G49
N3370 G05.1 Q1 R1
N3380 G43 H23 Z7.
N3390 Z1.9595
N3400 G01 Z1.7095
N3410 X-.1965 Z1.712
N3420 X-.1709 Z1.7262
N3430 X-.1636 Z1.7302
N3440 X-.1348 Z1.7426

 

 

That would work fine....

 

Force tool change is your friend here

[Newbeeee™]

This is the format we use for both 31i, OiMC and OiMD:-

 

%

O0657

( CUSTOMER )

( DESCRIPTION )

( DRG NO: )

( ISSUE NO: )

( OP NO: )

 

G17 G21 G40 G49 G69 G80 G90 M05

 

M00 ( NEW PROGRAM )

( USE BLOCK SKIP TO DISABLE G05.1 HSM )

 

(G54 DATUM)

G10G90L2P1X0Y0Z0

 

M1

 

N0101 T1 M6

M1

( 40MM DIA KORLOY FACEMILL )

( FACE TOP TO Z3.0. )

G10G90L12P1R20.

/G05.1 Q1

 

G54 G0 G17 G40 G49 G69 G80 G90 X72.998 Y85.5 S9000 M3

G43 Z25. H1

Z5.75

G1 Z3.5 F2500.

Y-45.5

G2 X43.799 R14.6

G1 Y45.5

G3 X14.6 R14.6

G1 Y-45.5

G2 X-14.6 R14.6

G1 Y45.5

G3 X-43.799 R14.599

G1 Y-45.5

G2 X-72.998 R14.599

G1 Y85.5

G0 Z25.

 

( FACE TO Z2.50 )

X0. Y81.

Z5.75

G1 Z2.5 F2500.

G41 D1 X-35.

G3 X0. Y46. R35.

G1 X67.

G2 X67.75 Y45.25 R.75

G1 Y-45.25

G2 X67. Y-46. R.75

G1 X-67.

G2 X-67.75 Y-45.25 R.75

G1 Y45.25

G2 X-67. Y46. R.75

G1 X0.

X1.

G3 X36. Y81. R35.

G1 G40 X1.

G0 Z25.

G28 Z25. M19

G05.1 Q0

G49

X0.

G28 Y81.

T1 M6

 

M30

%

 

We have the G49 in the cancel codes and then call at the very end of the path, just before a toolchange.

G49 is tool length compensation cancel - if you have it at the start before the G43, I think our machines didn't like it either.

So at then end is safest.

That said, ours is a custom post...

[Newbeeee™]

.DOUBLE POST - DOH!

[shredder]

I cant seem to find force toolchange in this post:(

[Guest]

Now I suggested the force tool change as it looks like this is a follow on operation with this tool

 

[shredder]

Thanks again

[shredder]

It worked gr8 jp thank you:)

[Guest]

You are quite welcome

[Allan]

There is a parameter that controls if G49 makes movement or not.

If set to not make movement their would be no issue as the height would be canceled (no movement) then apply high speed code.

When the Z is set to move the G43 call would be applied.

 

 

 

 

[Guest]

Change that parameter. :

[Newbeeee™]

^^^Foggy - you'll know the answer:-

For the Robodrills, would this parameter change have saved us having to put the G49 in the prog?

Our Chevalier's didn't need the G49 because the toolchange macro had it within.

So I faffed about with the Robo's to look at changing the toolchange prog, and realised it was a compiled/hidden one.

So I then faffed about more and via parameter changed to disable/ignore the standard toolchange and created a toolchange 9001 style prog thinking that we could use this (with a G49 within it of course) but then could not get the Robo to ignore the standard toolchange and read mine (although the parameters were set correctly).

So after a huge amount of faffing about I came to the conclusion that the Robo had compiled toolchange that could not be disabled/changed, so decided it was better to do a post mode to call the G49 (as above in my previous post).

 

So after typing this long winded question, am I now assuming that all I had to do was change a parameter 0 to 1 as per Alans statement and all would have been sweet and I could have been faff free LOL?