What's new
What's new

Haas multiple codes alarm

goins6720

Plastic
Joined
Jan 5, 2023
Keep getting a multiple code alarm trying changing stuff around but no progress

G71 P10 Q20 D.065 U.02 W.005 F.011
N10G42X1.36Z.1
G01 Z.02
X1.62 Z-.12
Z-2.19
X1.63
X1.771 Z-2.26
Z-4.87
X1.98
G03X2.Z-4.88R.01
G01 Z-5.35
N20 G01 G40 X2.15 Z-5.35
G00 X2.15 Z.1
 
What happens if you remove the G42 from the N10 block?

For what it's worth, whenever I want to program a roughing cycle with comp, I activate it BEFORE the G71 call and cancel it AFTER the Q block.
IOW the P-Q block does not have a comp within in it.
 
have you tried omitting g42 and see what happens.
the line before G3 could say ' X2.0 R.01 ' and dont use the G3 line. i assume you have several lines before the ones you posted, to start the prog. (like T0101 , G50, M3 ... etc,)
 
If G70 is going to be used after G71/G72/G73, there is no need to use radius compensation within the roughing cycle. The best is to insert G42 just before G70, and G40 in the following block.

Very few controls can use radius compensation within the roughing cycles.
 
Very few controls can use radius compensation within the roughing cycles.

Haas and Mits can use it, but care must be taken that the W value in the G71 block will be applied no matter what, and the part will be overcut.
To work around that you must alter the toolpath so the overcut is eliminated, which in turn makes the path useless for the G70 call.
But, that is also OK as G70 is normally useless anyway...
 
If the profile in non-monotonic, W has to be zero. Only U is to be specified.

G70 is useless only if the same roughing tool is used with it.
The idea is to use a roughing tool with G71/G72/G73, followed by a small-nose-radius finishing tool with G70. This would obviate the need for radius compensation in most cases.
Also. if radius compensation must be used, and roughing cycles do not allow, then G70 has to be used.
 
G70 is useless only if the same roughing tool is used with it.
G70 is always useless, but that is only from my own determination.
G71 and G72 is virtually essential in pretty much all applications, but the G70 following it is just shit.
Plain and simple!
G70 is useless!
 
What happens if you remove the G42 from the N10 block?

For what it's worth, whenever I want to program a roughing cycle with comp, I activate it BEFORE the G71 call and cancel it AFTER the Q block.
IOW the P-Q block does not have a comp within in it.
Seymour,

Would you mind posting a snippet of code where you do this?
I've not seen it that way before.
Thanks!
 
This one is for a 2" ball from a slug.
Rough ops are split. First, front up-to quadrant with a CNMG, then the back side with a VNMG.
It then finishes enough of the ball so it can be chucked up on the OD for the 2nd op to blend.


G28
G54
(OD ROUGH FIRST PASS - CNMG)
G50 S1200
G00 G97 T101 S500 M03
G00 X2.2 Z0.005
G96 S400 M08
G01 X-0.05 F0.005 (FACE TO .005)
G01 X2.15 Z0.05 F0.2
G96 S400 M08
G71 D0.08 P10 Q50 U0.008 W0.003 I0.01 K0.004 F0.008
N10 G00 X0.
G01 Z0
G03 X2. Z-1. R1.
G01 X2. Z-1.675
N50 G01 X2.15 Z-1.675
M09
(OD ROUGH SECOND PASS - VNMG)
G28
G50 S1200
G00 G97 T202 S500 M03
G00 G42 X2.2 Z-0.95
G01 X2.1 Z-0.95 F0.01
G96 S400 M08
G71 D0.04 P100 Q150 U0.008 W0.003 F0.008
N100 G01 X2. Z-1.01
G03 X1.4756 Z-1.685 R1.
N150 G01 X2.1 Z-1.685
M09
G00 G40 X2.3 Z-0.9
G28
(FINISH OD - VNMG)
G50 S1600
G00 G97 T404 S500 M03
G00 G42 X-0.4 Z0.2
G96 S600 M08
G01 X-0.4 Z0. F0.006
G01 X0. Z0. F0.002
G03 X1.6 Z-1.6 R1.
G01 X2. Z-1.6 F0.1
G01 G40 X2.4 Z-1.3
M09
G28
T101
M30
 








 
Back
Top