MAN READABLE COMMENTS, AND M00

[Larry1958]

I am having a problem trying to enter a program stop and output a comment for the operator to move clamps. I am using manual entry toolpath and setting dialog to NCI output "as code" but am still getting my (M00) as comment. I can edit the () out but if I forget then the tool may crash into a clamp. Any suggestions???

[Michael Sullivan]

I had this problem using an older post. The As code button did not make a difference. Are you running Version X?

Are you using an older version post that you updated?

 

If so, You need to edit your post to look like this:

 

pcomment2 #Comment from manual entry

scomm$ = ucase (scomm$)

if gcode$ = 1006, scomm$, E$

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

 

And of course, Make sure the "as code" box is checked!

[Larry1958]

Michael,

 

I am using X2, and yes it is a old post converted. I checked the post it is as follows

 

pcomment$ #Comment from manual entry (must call pcomment2 if booleans)

pcomment2

 

pcomment2 #Comment from manual entry

scomm$ = ucase (scomm$)

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

else, n$, "(", scomm$, ")", e$

 

I changed 1007 to 1006 as you have in yours and still get the same results.

[elbro]

Larry remove the (

 

if gcode$ = 1007, n$, scomm$,

[spade117]

Change the 1007 to 1006.

[Larry1958]

Actually I removed it from

 

else, n$, "", scomm$, "", e$

 

and it works fine. Thanks bunches guys.

[Colin Gilchrist]

Be very careful Larry.

 

If you change it so anything besides 1007 (which is what you have done) gets output as code, then your tool comments will not come out with the paraenthesis around them.

 

Do what Spade said, Change the 1007 to 1006, and leave the rest of the comments with the paraenthesis.

 

When you write a Manual Entry toolpath, be sure to enable the "As Code" option (this changes the NCI output from 1005 to 1006).

 

Good luck,

[Ocean Lacky™]

 

 

I find this easier than post editing

[Colin Gilchrist]

But that forces a tool change Ocean. The Manual entry works great once you tweak your post.

[Ocean Lacky™]

Colin, If you're using the same tool, there is no change, it just moves the spindle back out of the way for the operator to go and do their thing.

 

[buttkiss] It's just one of many options, which is what makes Mastercam so great! [/buttkiss]

 

[Randy Morton @ Clem Industrial]

Larry,

 

Why not use MI's? I have customized a whole heap of them to output at certain locations when I turn them on (using 1, 2 or whatever number you want). You can get really specific with their placement as well. If you run out of MI's you can double up.

 

I can't remember the exact syntax since I am at home, but something like this;

 

IF MI1 = 1, "MOO"

IF MI1 = 2, "M00 (CHANGE CLAMPS)"

IF MI1 = 3, "M01 (YOU JUST MACHINED THE CLAMP)"

 

Or something of the similar. Again, you could assign each to a different MI until you use them all up.

 

Very useful. Personally I find it more useful then manual entry (although that has a few cases of use too...)

 

JM2C

[Henk]

quote:

---

MI's:

Very useful. Personally I find it more useful then manual entry (although that has a few cases of use too...)

---

My PLUS for the Manual Entry is that you can see them in the toolpath-manager, the MI's are hidden in the prameters.

[Dan@home]

Collin; I have made the change from the 107 to 106. On both posts, (old and updated) why both posts are there I don't know. I still get ( ) around everything.

[foolsh]

Just use the simple canned text!

[Dan@home]

Michael.su; That worked for me..

 

Dan.

[Guest CNC Apps Guy 1]

quote:

---

...IF MI1 = 1, "MOO"...

---

That's gonna give you problems.

 

It needs to be IF MI1 = 1, "M00"