N at the beginning of each tool?

[gearsoup]

From what I've seen, it only appears that MCAM will let me either ouput sequence numbers for the entire program, or none at all. Is it possible to have it spit out an N code at the startup block for every tool? Example of what I want:

N10G0G40G80G90G94G98
M01
T1M6
G0G90G54X-1.125Y-.25S6112M3
G43H1Z.25M8T2
G4 P1000
Z.1
G1Z0.F48.9
G41D51X-.875F97.79
G3X-.625Y0.R.25
G2I.625
G3X-.875Y.25R.25
G1G40X-1.125
G0Z.25
M9
G91G30Z0.M19
M01

N20G0G40G80G90G94G98
T2M6
M01
G0G90G54X-.1875Y.125S10000M3
G43H2Z.25M8T3
G4 P1000
Z.1
G1Z0.F97.79
G41D52X-.3125F195.58
G3X-.4375Y0.R.125
I.4375
X-.3125Y-.125R.125
G1G40X-.1875
G0Z.25
M9
G91G30Z0.M19
M01

N30G0G40G80G90G94G98
T3M6
M01
G0G90G54X0.Y0.S9167M3
G43H3Z.1M8T1
G4 P1000
G99G81Z0.R.1F88.
G80
M9
G91G30Z0.M19
G28Y0.
M30
%

why does everything go to lowercase?

[Switcher]

why does everything go to lowercase?

The whole forum is messed up (lowercase).

.

[Mike Mattera]

Find the section in the post that you want the output. Most likely this will be the ptlchg section of the post. Find the line where you want to force out the block number. Find the "n," in that line and replace it with a *n, "n" is the variable for the block number and the * forces the output of that variable. Then make sure the omitseq variable is set to yes (or 1).

You you've turned off block numbers, except for that one place where you're forcing them out.

Mike Mattera

[gearsoup]

Thank you! I'll give it a shot.

[gearsoup]

Originally Posted by Mike Mattera Find the section in the post that you want the output. Most likely this will be the ptlchg section of the post. Find the line where you want to force out the block number. Find the "n," in that line and replace it with a *n, "n" is the variable for the block number and the * forces the output of that variable. Then make sure the omitseq variable is set to yes (or 1). You you've turned off block numbers, except for that one place where you're forcing them out. Mike Mattera

So, I've tried that, and it's not working. I found the n$ before the beginning of each toolchange, changed it to a *n, and it still posts out as:
G0G40G80G90G94G98
This is at the beginning of each tool, and I would like it to add in a "N10", or "N20", whatever tool # I'm on....

[gearsoup]

omitseq$ : yes$ #CD_VAR Omit sequence numbers? seqmax$ : 9999 #CD_VAR Max. sequence number

pbld, *n, *sgcode, scc0, sg40, sg80, *sgabsinc, sg94, sg98, e$

This is what I've got in my post....

[Mike Mattera]

Did you say you were using MCam X? No.

Put the *n$ in and try it again.

It aways helps when you tell us what version your using.

Mike Mattera

[gearsoup]

Mike,

Thank you! That works now. Sorry about not mentioning what version I was using. I wasn't aware that made a difference....

One last question, if I may.... It gives me N100 at T1, N102 at T2, N103 at T3, etc. etc. Now do I get it to do N10, N20, N30, N40, etc. etc. I set the increment in the control definition to 10, but that doesn't seem to make a difference.

[Mike Mattera]

Machine Type - Control Definition - NC-Output - Start Seq Num = 10 - Increment Seq Num = 10.

Mike Mattera

[gearsoup]

I'll be darned. That did it. I had changed it just in the control definition. Apparently, one needs to go into machine def. and then into control def. and then re-load the machine def.... thank you!