Make machine stop and wait?

[SpazMachine]

I need some advice on the easiest way to do this. On my mill I have some Erowa pallete system holders. Most of the time the part needs to be rotated a few times before it's done. In the past I have just loaded a new program every time I rotated it. I want to post the whole thing and have the mill stop and prompt to rotate the part the correct way. What's the easist way to pull this off? I have tried putting a manual entry at the top of every new group of programs. It's getting close.

 

%

O0000 (Z.NC)

(TOOL - 6 DIA. - .125)

N100G20

N102G0G17G40G49G80G90

M00

(G55 EROWA DOWN)

N104T6M6

/N106G106T6

N108S12000M3

N110G05 P10000

N112G55G00 X0 Y0

N114G43H6Z6.

N116M46

N118G0G90X-2.0884Y-3.0349

N120G1Z.35F40.

N122X-2.0259Y-2.7724F80.

 

...

 

N456X-1.1624Y-1.8084Z-.015

N458G0Z6.

M00

(G55 EROWA UP)

N460X2.0884Y-3.0349

N462G1Z.35F40.

N464X2.0259Y-2.7724F80.

 

...

 

N258X1.1078Y-1.7305Z-.015

N260G0Z6.

N262M5

N264M47

N266G05 P0

N268G91 G28 Z0

N270G91 G28 X0 Y0

N272M99

%

 

 

Problem is, I need the mill to go g28 z0 x0 y0 to get out of the way and then do all the right steps to get back where it came from. Maybe stick a tool change in there or something. I don't know. What's easier?

[Lathe-Mill]

force tool change

operations manager, select the tool path, click on change nci , then check force tool change

[Eric S.]

Hello

 

You can change your post to output a M00 before the operation using the miscellaneous values.

[Avs_Fan]

quote:

---

force tool change

operations manager, select the tool path, click on change nci , then check force tool change

---

Hi Lathe-Mill,

Nice tip, thanks for sharing!

I didn't know that one, but got to try it today.

My previous way to do this was to use a duplicate tool with a different # & then manually edit tool #s.

There's always something new to be learned on the Forum.

[Lathe-Mill]

your welcome,glad i could help

[SpazMachine]

Alright. It's almost kind of working now. I still have a few things to work out. The tool change doesn't move the machine up and out of the way. It doesn't add G28's in there anywhere It's up to the tool change program in the mill to do those and if it is changing to a tool it already has it just blows them all off. I think I can cram them in the post somewhere.

 

As long as I'm in there does anyone know how to make the post output a space between each word in the program? It is a lot easier to read that way.

[medaq]

Toolpaths, next menu, manual entry. click 1005 option, and type what you want it to read.

 

My pcomment2 has to look like this to make it work though..

 

pcomment2 #Comment from manual entry

scomm = ucase (scomm)

if gcode = 1005, scomm, e

if gcode = 1006, "(", scomm, ")"

if gcode = 1007, "(", scomm, ")"

else, "(", scomm, ")", e

 

Jim

[medaq]

Btw use the manual entry in conjunction with the force tool change. Does miracles

 

I do alot of g10 off sets. So I use manual entry at the begining of the program to force my offsets and work offsets in.

 

Jim