[solidcam2011ls]

Hi all

can any one see anything wrong with my gcode please see below , im trying to apply g68 - g69 workoffset rotation with my probe. but when i have s1 in the corner measure macro call it dont apply rotation and cuts on an angle. but if i take out s1 it seems to work.

Do i have to measure my stock twice one for workoffset and one for rotation???

T30(PROBE)
M6
G0G54X-10.00Y-10.00M19(SET G54 G55 ETC SET X Y)
G43Z50.0H30
M600(TURN ON PROBE)
G65P9810Z-10.00 F500(PROTECTED MOVE SET Z)
G65P9816X0Y0I40.J40. S1(external Corner find)
G65P9810Z10.00(PROTECTED MOVE)
G65P9810X10.00Y10.00(PROTECTED MOVE SET Z)
G65P9811Z0S1(SET G56 Z)
(Z0 WILL BE 0MM FROM TOP OF JOB)
(Z1 WILL BE -1MM FROM TOP OF JOB)
G65P9810Z10.00(PROTECTED MOVE)
G65P9810Z50.F2000
M601(TURN OFF PROBE)
(------------------)
(STOP PROBE OP WEB)
(------------------)
G05.1 Q0 (SMOOTH INTERP/BLK LOOK AHEAD Off)
G0 G28 G91 Z0 M9 (COOLANT OFF)
G30 X0 Y0 M5 (SPINDLE STOP)
G90 (ABSOLUTE PROGRAMMING)
M25(CONVEYOR STOP)
M01 (OPTIONAL STOP)

N1 T14 M6(TOOL -14- MILL DIA 6.0 R0. MM )
G0 G40 G56 G80 G90 G94 G98 X50. Y120.61 S10000 M3
M24(CONVEYOR START)
G43 Z50. H14 T14 M08 (COOLANT FLOOD)
G68X#135Y#136R#139 (Offset Rotation ON)
(---------------------)
(FIRST POCKET - POCKET)
(---------------------)

[christinandavid]

Isn't S1 for setting G54? Your program calls G56...

DP

[solidcam2011ls]

I didnt notice that im stupid I will give it ago with S3 not sure if this will stop my workoffset rotation. as i think the probe can only save one set of values to use but I may be wrong. It may be that the probe saves the values for g54 g55 etc I will test it tomorrow. thanks

[christinandavid]

My advice with Renishaw problems is to get straight in touch with user 'guypb' via this site.

DP

[renrepjnr]

100 series variables are over written when you call up different probing routines. If you want to find a corner and angle and not apply it right away you should copy the value(s) to different location(s) so they are not overwritten when you call up the 9811 or other routine(s)... Exp. #189=#139 and since you are updating the work offset to the corner call G68X0Y0R#189 or the free variable you choose to store the angle in.

[guypb]

My advice is to go with renrepjnr, your 9811 cycle is overriding the common macro variables created in your 9816 which you need for your G68.


G65P9816X0Y0I40.J40. S1(external Corner find)
#189=#139 (STORE MEASURED X ANGLE)
G65P9810Z10.00(PROTECTED MOVE)
.... (all other code here)
G68X0Y0R#189

This would work as you have already updated your X0.Y0. with the S1 in the 9816 anyway.

[solidcam2011ls]

thanks for all the help I will give it a shot as soon as i can
im learning more stuff from this site and you lot everyday.

I have never used variables before only the standard renishaw stuff, how would i find out what variables are not being used. sorry if this is a stupid question i am new at all this.

thank you all again.

[guypb]

Inside the Inspection Plus manual, there is a "variable map" which shows you which Renishaw cycles use which variables. The appendices also talk in greater depth about ALL the Renishaw probing cycle assignments.

For calculations you will find that nested local (#1-#32) variables and lower common (#100-#149) variables are used. Some controls also have extended common variables (#150-#199). These variables are normally considered "fair game" - as in they are not usually used for long term storage and only for calculation or flag purposes within the macros themselves.

There are then other common variables (#500 - #549) which are used for storage (like probe calibration data). Again on some controls these are extended to #599, #699 or even #999. It is easy to use these variables for storage but I strongly suggest mapping what you want to put and where to make sure a) you don't overwrite something critical b) you know which variables can be re-used.

Hope this helps!