Manual Entry for M0 program stop??

[ddelauter]

I have been looking for a way to add a program stop through the Operations List, but when I do it allways puts parenthesis "()" around the codes, and the machine won't read it as a command.

I basically want to have the program stop and table movement automatically entered into the NC code every time I post, rather than entering it manually every time.

This is the code I would like to have automatically entered:

G28Y0

M0

I would like to put that before or after whatever operation I want, through the operations list.

Any help is greatly appreciated. Thanks in advance..

Don

[Rekd™]

I've got one set up using misc values. It only goes before the operation that it is assigned to. It will also prompt you for a comment to place with the M0. It has the tool change info, that works with null tool changes as well as normal tool changes. Changing the Y move will be easy.

Here's a sample of the code:

N244 G00 Z1.

N245 M05

N246 G49 Z0.

N247 G59 Y-4.

N248 G54

N249 M00 ( ENTER COMMENT HERE )

N250 (FINISH POCKET)

N251 T2 M06 (3/4 FLAT ENDMILL 0.75)

If you're interested, let me know and I'll send you the post data.

Rekd

[ddelauter]

thanks for the help, but I think I have found what the problem was.

In my post, the code for manual entry was as follows:

pcomment # Manual Entry - COMMENTS (on a block by itself) 1005,1006

"(", scomm, ")"

I just took out the quotes and parenthesis.

BTW, if anyone knows if this will cause a problem please let me know ASAP!!!

[cadcam]

as long as you dont put any thing eles you should be fine.

but now mastercam puts coments in the comments window for you so you need to watch every time you write a program, that it did not post some thing for you.

all it takes is the wrong letter and BOOM the machine CRASHS..

so i suggest you follow REKD and look at what he is offering.

truefulyu i would like to see it, if he do's not mind.

then if he would like i can put on my FTP to share if he would like.

------------------

jay/ aka cadcam

Precision Programming

cnc programming &

Predator reseller

email: [email protected]

web: www.ppcadcam.com

[ddelauter]

i have tried it a few times with no problems. I am just using a text file that has been tested, so as not to have a typo-error.

G28Y0

("ENTER COMMENTS HERE")

M0

Thanks all for your help, this is what I wanted.

[Rekd™]

Jay,

I emailed you the code I use for the program stop. I think I got everything..! If not, lemme know.

The post I made for this has a few other 'goodies' that you could prolly live without, but I find very useful. Like a drill cycle made for a drop-stop; really useful if you ever use a dowel pin in the spindle to locate parts, does it automatically, just like drilling holes.

Haven't figured out how to safely get rid of the G80, but it's not gonna hurt anything there.

N2 G00 G17 G40 G49 G80 G90

N3 (LOCATE X0)

N4 T3 M06 (.250 TOOL STOP)

N5 (DEPTH: Z-.25)

N6 G00 G90 G54 X-.125 Y1.

N7 G43 H3 Z1.

N8 X-.125 Y1.

N9 Z-.25

N10 M00

N11 Z1.

N12 G80

N13 M05

Enjoy!

Rekd

[cadcam]

thank vary much got it.

i like it and going to put it in sevral of my post..

------------------

jay/ aka cadcam

Precision Programming

cnc programming &

Predator reseller

email: [email protected]

web: www.ppcadcam.com

[kathy]

Hi,

I have a pstop sequence in my posts that I tag with using Misc Variable 10. If I want to stop a tool between contours, I break the contours into a definate start / stop, and place a point on the start of the second contour. In the point's parameter, I eval MV 10 = 1. This inserts a pstop sequence (retracts and stops tool, moves table forward to home, and add tools start stuff after pstop) from my post(example Fadal):

pstop # program stop

n, "G00 G49 M47 Z0 M5", e

n, "E0 X0 Y0", e

n, "M00( PROGRAM STOP)", e

pss, e

n, "E1", *xr, *yr, e

n, ptllncomp,e

mi10=0

I also use a similar sequence when pstoping at a tool change.

Kathy