Haas Post

[PORT]

Why, when starting a new toolpath does the post start at the previous toolpaths last X,Y position then rapid to the new toolpaths position to start machining. Here is a sample.

Would like line 250 to be the same as X,Y as line 280.

 

Thanks,

Nick

 

%

O0

(PROGRAM NAME - TEST )

N100 G20

N110 G0 G17 G40 G49 G80 G90

( CENTER DRILL TOOL - 10 DIA. OFF. - 0 LEN. - 10 DIA. - .25 )

N120 T10 M6

N130 G0 G90 G54 X-1.5 Y.1245 S3000 M3

N140 G43 H10 Z.1

N150 M8

N160 G99 G81 Z-.06 R.1 F10.

N170 X0.

N180 X1.5

N190 G80

N200 M5

N210 M89

N220 G91 G28 Z0. M9

N230 G28 Y0. M84

( 17/64 HSS DRILL TOOL - 11 DIA. OFF. - 0 LEN. - 11 DIA. - .265 )

N240 T11 M6

N250 G0 G90 G54 X1.5 Y.1245 S1000 M3

N260 G43 H11 Z.1

N270 M8

N280 G99 G83 X-1.5 Y.1245 Z-1.5249 R.1 I.25 J.1 K.125 F4.

N290 X0.

N300 X1.5

N310 G80

N320 M5

N330 M89

N340 G91 G28 Z0. M9

N350 G28 Y0. M84

( 5/16 TAP OSG TOOL - 12 DIA. OFF. - 0 LEN. - 12 DIA. - .3125 )

N360 T12 M6

N370 G0 G90 G54 X1.5 Y.1245 S324 M3

N380 G43 H12 Z.1

N390 M8

N400 G99 G84 X-1.5 Z-1. R.1 F18.

N410 X0.

N420 X1.5

N430 G80

N440 M5

N450 M89

N460 G91 G28 Z0. M9

N470 G28 Y0. M8

[Guest]

What does your ppeck$ section in your post look like?

[PORT]

ppeck$ #Canned Peck Drill Cycle

pdrlcommonb

pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, *peck1$, *feed, strcantext, e$

pcom_movea

 

This porblem is not just on canned cycles. It even happens on a simple contour program when ever there is a tool change.

[Guest]

New problem?

 

What post are you using?

 

Is this an updated post to VX?

[Storkman]

ppeck is outputting the correct info, I would think the problem is in ptlchg_com.

[PORT]

I think you maybe right Storkman. It is a Haas post that was updated from 9. This is a new problem that has potential to crash a tool . Had this problem in 9 before, but not involved in the change.Here is a copy of the post.

 

ptlchg #Tool change

pcuttype

toolchng = one

if mi1 = one, #Work coordinate system

 

 

pcom_moveb

c_mmlt #Multiple tool subprogram call

ptoolcomment

comment

pcan

pbld, n, *t, "M6", e

pindex

sav_absinc = absinc

if mi1 > one, absinc = zero

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs, pfxout, pfyout,

pcout, *speed, *spindle, pgear, strcantext, e

pbld, n, "G43", *tlngno, pfzout, next_tool, e

pbld, n, scoolant

absinc = sav_absinc

pcom_movea

toolchng = zero

c_msng #Single tool subprogram call

[robk]

PORT, see if this will make a difference...BTW, back up your post before making any changes...

 

 

ptlchg #Tool change

pcuttype

toolchng = one

if mi1 = one, #Work coordinate system

[

pfbld, n, *sg28ref, "X0.", "Y0.", e

pfbld, n, "G92", *xh, *yh, *zh, e

]

pcom_moveb

c_mmlt #Multiple tool subprogram call

ptoolcomment

comment

pcan

pbld, n, *t, "M6", e

pindex

sav_absinc = absinc

if mi1 > one, absinc = zero

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs, pfxout, pfyout,

pcout, *speed, *spindle, pgear, strcantext, e

pbld, n, "G43", *tlngno, pfzout, next_tool, e

pbld, n, scoolant

absinc = sav_absinc

pcom_movea

toolchng = zero

c_msng #Single tool subprogram call

[Roger Peterson]

PORT, robk is right on. The post block pcom_moveb calculates absolute and incremental values. The way your post was setup it was only going to calculate those positions if mi1 = one. Placing the code in that robk outlined will take pcom_moveb out of the if mi1 = one boolean operation. Someone removed the code without knowing what the consequences were.

[PORT]

Thanks, works like it should now. Really appreciate the help from all.

 

Nick