How can I force a Z move before XY in post?

[Bill]

I have been using an old hurco post for my old machines. Now we have a new Hurco and it will not move Z to safe position before cycle start or at cycle start like the old machines.

 

I think it is hard coded in the old ones.

 

Anyhow... I will get an X Y position call out before a Z and the foreman smashed the cutter and knocked the piece out of the vise last night by not knowing what he was doing.. Funny story check O/T. SMASH.

 

Here is an example of the code and notice the weird H0 callout for T1 also. That looks wrong to me.

 

N150T1M6

N160G0G90X-1.353Y-3.4774S2750M3

N170G43H0Z5.

 

Thanks guys. Don't know what I'd do without this forum and everyone's help.

[Guest]

biilh,

 

Are you using X?

 

If you are the H0 could be cause by the control def.

 

If you need T1 H1

 

Check in the control def >> tool fromt he tool offset register to make sure you are set "add to tool" 0 & 0

 

On you Z height problem, what do you get for code and what are you looking to see?

[Bill]

John yes i am in X.

 

I will check that. This is a new post the Hurco guy sent me from 9.1 so I hadn't reveiwed the con def yet. My old def was for the old hurco post and it was set like that. Thanks for the reminder.

 

As far as output, I would like to see the Z move before the X Y at the start of the program because... look in O/T and see smash. Pretty funny.

[Guest]

DO you want to hard code a G91 G28 Z0 just at the begining of your program?

 

To do that go into the psof$ section and add roght before your saftey block this

 

code:

---

pbld, n, *sg91, "G28", "Z0.", e

---

[dwsz71]

Could you hard code a move to home position before the first tool change:

 

code:

---

 %

O0001 ( I210-141904 - METRIC BOTTOM INSIDE GUARD )

( REVISION A ) ( MILL OP. 1-1 )

( LOAD 210/141904-M1.NC )

N5 G00 G17 G20 G40 G49 G80 G90

N10 G28 G91 Z0.0

N15 G28 X0.0 Y0.0

( #4 CENTER DRILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .3125 )

( CENTER DRILL HOLES )

N20 T01 M06

N25 G00 G54 G90 X-5.75 Y-0.375 S1925 M03

N30 G43 H01 Z1.0 T02

---

I'm not familiar with Hurco posts at all, so I don't know if this is even an option for you. It would need to be added to the psof$ or maybe the pheader$ section of the post.

 

I would also have at least the "G28 G91 Z0." at the begining of the next tool change. Of course, this is because I need it for tool changes.

 

As for the H0 I would double check the Op. Params.

 

HTH

[Bill]

Yes if Z 0 would be machine home.

 

Also I checked and I had con def set to "from tool" and the tool number is 1 so the H should be 1 as well in the post I would think.

[Bill]

this is my psof.

 

psof #Start of file for non-zero tool number

pcuttype

toolchng = one

if ntools = one,

[

#skip single tool outputs, stagetool must be on

stagetool = m_one

!next_tool

]

"%", e

*progno, e

"(PROGRAM NAME - ", sprogname, ")", e

"(DATE=DD-MM-YY - ", date, " TIME=HH:MM - ", time, ")", e

pbld, n, *smetric, e

pbld, n, *sgcode, *sgplane, "G40", "G49", "G80", *sgabsinc, e

sav_absinc = absinc

if mi1 <= one, #Work coordinate system

[

absinc = one

pfbld, n, sgabsinc, *sg28ref, "Z0.", e

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

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

absinc = sav_absinc

]

pcom_moveb

c_mmlt #Multiple tool subprogram call

ptoolcomment

comment

pcan

if stagetool >= zero, pbld, n, *t, "M6", e

pindex

if mi1 > one, absinc = zero

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

pfcout, *speed, *spindle, pgear, strcantext, e

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

absinc = sav_absinc

pcom_movea

toolchng = zero

 

I would think it needs to be added here

[Guest]

You could add the line I posted above right after the *progno, e

 

will look like

 

*progno$, e$,

pbld, n$, *sg91, "G28", "Z0", e$

[Bill]

the $ signs are missing CUZ its early and that was copied from the V9.1 post. Doh!

[Bill]

Gotcha thanks guys.

 

Will give it try and see what it looks like.

 

One more question if I may. the smetric$ what is that doing? Like I said I got this from a dealer and I do not use metric, will that be an issue?

[Guest]

nO, that checks to see if you are in metric an outputs the correct code, either G20 or G21

 

G20 is Imperial

G21 is Metric

[Bill]

I see the G20.

 

Here is the ouput I get now by adding that.

 

N100G20

N110G0G17G40G49G80G90

/N120G91G28Z0.

/N130G28X0.Y0.

/N140G92X10.Y10.Z10.

(MILLSTAR 1 1/4 BULL CUTTER WIH 6MM RAD TOOL - 1 DIA. OFF. - 0 LEN. - 0 DIA. - 1.25)

N150T1M6

N160G0G90X-1.353Y-3.4774S2250M3

N170G43H0Z5.

N180Z4.75

 

Does the forward slash null the block?

[Steve Biehl - Cimquest Inc]

The / is caused by the pfbld sections. The f in pfbld stands for 'Forced'. Take the f out and you'll be fine.

[Bill]

Looks like that is what I needed.

 

It weird the older machine has it hard coded in to retract Z to home on Cycle start.

 

Oh well.

 

Thanks John.

 

I will try to figure out that H0 callout now.

[Bill]

The H0 callout was caused by my tool #1 had a length offset = to 0

 

H was looking for the length offset.

[Bill]

Ok thanks Steve.