Need a change to a post

[PAnderson]

Can someone please help me add a G90 to this attached post. It does a G91 G28 Z0. at the beginning and at every tool change but does no add a G90 after. I cannot find the spot to add the G90. After every tool change, the Z Axis wants to over travel. Thanks in advance.

Paul

O0000
(TEST)

(MATERIAL - ALUMINUM INCH - 2024)
(T1|3 BULL-NOSED ENDMILL|H1|D1| DIA. - 3.)
G20
G0 G17 G40 G49 G80 G90
G0 G28 G91 Z0.
(3 BULL-NOSED ENDMILL|TOOL - 1|DIA. OFF. - 1|LEN. - 1| DIA. - 3.)
M11
M39
T1 M6
G0 G54  X4.1 Y0. C0. A0. S3056 M3 ( I need a G90 on this line and after every tool change )
M10
M38
G43 H1 Z2.
X4.1 Y0. Z2.
G90 Z.2

Doosan DNM 200-5AX MILL_G68.pst

[Guest]

pbld, n$, *sgcode, pwcs, *sgabsinc, pfxout, pfyout,
        [if nextdc$ <> 7, *speed, *spindle], pgear, e$ 

the *sgabsinc should get you if you add it to the line that is outputting

[nickbe10]

If it is MPMASTER another solution is to move the output line for the z clearance:

pbld, n$, "G00 G91 G28 Z0.", e$

ahead of the output line for the safety line:

pbld, n$, *sgcode, *sgplane, *smetric, "G40", "G80", *sgabsinc, e$

I like this because the first thing it does is get the spindle out of potential trouble area, especially for inexperienced operators, then reads the safety line to start the program and you are automatically in G90 and ready to go.

So I get this at the top of every prog:

G00 G91 G28 Z0.
G00 G17 G20 G40 G80 G90

 

[PAnderson]

JParis,

That worked. Thank you so much. I knew the code, I just did not know where to place it so that it would work for the beginning of the program and at every new tool change.

 

Regards,

Paul