Excessive indexing

[John Morris]

Excessive indexing

 

I do a fair bit of simple 3 face work on our horizontals and usually create 3 work planes with the part approximately where it will be on the tombstone and initiate a safety zone to make sure the tools clear on indexes. One issue I am having is the code will come out with what I consider to be strange moves. For example it will choose to go A90. then to A270 instead of A90 and A-90. Then with it in position at A270 it will go to tool change, come back and wrap all the way back around to A-90. I’ve been looking through the machine definition and configuration files trying to find a switch or setting to at least get rid of the A270. to A-90 (same face) with an unnecessary 360.

 

Can anyone give me a good place to look or is this a post edit or even tell me if it is something within the model that I can control?

 

Thanks

 

Sample code below:

 

%

O5192

(DATE - 04-20-11)

( T3 | 3/8 SPOT DRILL | H3 )

( T43 | 1/8 DRILL | H43 )

( T44 | NO. 6-32 TAPRH FORM | H44 )

G20

G0 G17 G40 G49 G80 G90

( SPOT RIGHT )

( 3/8 SPOT DRILL )

T3 M6

G0 G90 G154 P5 A90. X-.174 Y0. S5093 M3

G43 H3 Z10. M8 T43

G98 G82 Z-.07 R.1 P.5 F10.19

G80

Z10.

( SPOT LEFT )

G154 P6 A270. X.174 Y0. Z10. ( WHY NOT A-90.)

G98 G82 Z-.07 R.1 P.5 F10.19

G80

Z10.

M5

M9

G91 G28 Z0.

A0.

M01

( DRILL B4 TAP 1/8 LEFT )

( 1/8 DRILL )

T43 M6

G0 G90 G154 P6 A-90. X.174 Y0. S11000 M3 (SHOULD STAY AT A270. !!!!!!!)

G43 H43 Z10. M8 T3

G98 G83 Z-.7476 R.1 Q.1 F20.

G80

Z10.

( DRILL B4 TAP 1/8 RIGHT )

G154 P5 A-270. X-.174 Y0. Z10. (THEN BACK TO A90. ???)

G98 G83 Z-.7476 R.1 Q.1 F20.

G80

Z10.

M5

M9

G91 G28 Z0.

( 6-32 TAP RIGHT )

( NO. 6-32 TAPRH FORM )

T44 M6

G0 G90 G154 P5 A90. X-.174 Y0. S300 M3

G43 H44 Z10. M8 T27

G98 G84 Z-.6 R.1 F9.375

G80

Z10.

( 6-32 TAP LEFT )

G154 P6 A270. X.174 Y0. Z10.

G98 G84 Z-.6 R.1 F9.375

G80

Z10.

M5

M9

G91 G28 Z0.

M30

%

 

X5 Mill level 2

[K2csq7]

What kind of post, machine def, control def are you working with?

[John Morris]

I'm using the standard Haas post that came with MC that was modified by our vendor to suite our request when we first got setup with Mastercam and it has been imported by each new version ever since.

[André Lapointe@In-House Soluti]

Hi John,

I think it may be a post configuration issue.

If you look inside the PST file and search for the following line:

frc_cinit : yes$ #Force C axis reset at toolchange

try changing its value to no$ so this way it won't reinitialize itself for the angle calculation at the toolchange. therfore getting rid of the unwanted 360 degres move.

 

HTH

[John Morris]

Thanks André,

 

That seems to fix the 360 problem. I need to do some further testing to see what effect that may have on axis sub programs (wrapped geometry).

[André Lapointe@In-House Soluti]

When this variable is on it is supposed to only affect the the rotary axis position at the toolchange sequence, so I'm pretty sure it won't change anything into your axis substitution toolpath.