misc values, G54/G55???

[chad fisher]

i have a haas post that our local reseller set up to use the misc values so i could post for different fix offsets. What i do i is on the first op is set it for 54 then copy and paste that opp

then set misc value to 55,.............boom posted for two vices, it has worked alright yesterday

now when i tried to post, the last opperation was suspose to move to g55 when it got done with 54 but it posted no xy movement. Maybe i am real ignorant here but personal opinion says that for simply posting for more fixture offsets is rather cumbersome. Any ideas would greatly be appreaciated. Thanks in advance

 

(PROGRAM NAME - 51 )

(DATE=DD-MM-YY - 29-10-02 TIME=HH:MM - 07:36 )

N100 G20

N102 G0 G17 G40 G49 G80 G90

( TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .15 )

N104 T1 M6

N106 G0 G90 G54 X-3.2 Y.06 S2546 M3

N108 G43 H1 Z2.

N110 M8

N112 G54 Z.1

N114 G1 Z-.075 F12.

N116 G41 D1 X0. F12.8

N118 G2 X.06 Y0. I0. J-.06

N120 G1 Y-2.25

N122 G2 X0. Y-2.31 I-.06 J0.

N124 G1 X-3.2

N126 G2 X-3.26 Y-2.25 I0. J.06

N128 G1 Y0.

N130 G2 G40 X-3.2 Y.06 I.06 J0.

N132 G0 G54 Z2.

N134 G55 "NO MOVEMENT???????????????????????????????????????????????

N136 G55 Z.1

N138 G1 Z-.075 F12.

N140 G41 X0. F12.8

N142 G2 X.06 Y0. I0. J-.06

N144 G1 Y-2.25

N146 G2 X0. Y-2.31 I-.06 J0.

N148 G1 X-3.2

N150 G2 X-3.26 Y-2.25 I0. J.06

N152 G1 Y0.

N154 G2 G40 X-3.2 Y.06 I.06 J0.

N156 G0 G55 Z2.

N158 M5

N160 G91 G28 Z0. M9

N162 G28 Y0.

N164 M30

%

[chad fisher]

Well to answer my own question i didnt have lead in and lead out checked, my morning ignorance prevails again! But why would it have not put any x y movement in the line that i marked??

[Allan Brown]

There are some other options in the tranform toolpath parameters to work with multiple offsets for identical parts. Search the forum for MPSUBREP_NEWMETHOD and Mpsubrep. These two techniques may help to avoid this situation.

[Roger Martin from CNC Software]

Chad,

 

Modality - that's why.

 

Look at the X,Y axis positions at the end of the 1st contour. They are at the SAME coordinates that the 2nd contour starts at. So, the post does not need to state the X,Y - because it is already there. Changing work offsets here is what changes the situation. You would want to re-state those X,Y coordinates. This would require a fairly simple post change to force output of the X,Y coordinates whenever the programmmed work offset changes.

[P_Scott]

Chad,

 

Did you move your geometry or just Copy the operation and change the input for the G55? That could be another reason for not getting different output in the code. Do a search for work offsets in this forum and you will find some useful information. HTH

 

[ 10-30-2002, 10:17 AM: Message edited by: Peter Scott ]