Blocknumber without N or +

[arsson]

I use X3 and mpheid5 posts mill.

My machine whant block number without N and no decimal.

When I set the box "output sequence number" in CD I got block number like this

 

0 BEGIN PGM 51 MM

+1.000 TOOL DEF 1 L+0.000 R+25.000

+2.000 TOOL CALL 1 Z S500.000

+3.000 L X-40.500 Y+77.000 R F1000 M

+4.000 L Z+25.000 R0 F1000 M03

+5.000 L Z+17.000 R F600 M

+6.000 L Y+52.000 R0 F300 M

+7.000 CC X-13.500 Y+52.000

+8.000 C X-13.500 Y+25.000 DR+ R F M

+9.000 L X+13.500 R F M

+10.000 CC X+13.500 Y+0.000

 

The correct results is

 

0 BEGIN PGM 51 MM

1 TOOL DEF 1 L+0.000 R+25.000

2 TOOL CALL 1 Z S500.000

3 L X-40.500 Y+77.000 R F1000 M

4 L Z+25.000 R0 F1000 M03

5 L Z+17.000 R F600 M

6 L Y+52.000 R0 F300 M

7 CC X-13.500 Y+52.000

8 C X-13.500 Y+25.000 DR+ R F M

9 L X+13.500 R F M

10 CC X+13.500 Y+0.000

 

Have you ansver?

 

Before i use MC9 it works fine.

 

My english is bad sorry

[Jim Evans from CNC Software]

Without seeing the post it is hard to say, but seeing you said it worked in V9 I'll take a stab at it.

 

IS this the first time you've run the post in the X platform? If so, please check your .err file for information. the .err file will be in the the same location as the NC file.

 

From the looks at the output I would guess that there is a problem line or lines in the post that when you updated everything to X the updatepost found problems and modified the bad line(s) trying to address the problems, but it was obviously unsuccessful. You can look in your post for the following code

code:

---

 #CNC<<CONVERT>> 

---

These are the lines from the V9 post that are not valid in X and will need to be fixed.

 

I'm guessing somewhere along the line the FMT assignment for N or the lines around it had problems and should have the #CNC<> around them or will show up in the .ERR file.

 

You can refer to the MAstercam Transition Guide in your documentation folder for more information on updating the posts.

 

If you find #CNC lines in your post or you have errors in your .err file after posting you can post them here and that might help point me in the right direction.

 

You also may want to create a zip2go file and send it off to your reseller for some help, because without the files you are going to just get guesses here.

[Josh T™]

Sounds like a bad format statement...

 

I'll check my Heidenhain posts and get back to you tomorrow or tonight.

 

Josh

[arsson]

No error in error log you can see.

But it change

" Post variable 'omitseq$' was re-initialized from 1. to 0."

I Test to change it to yes but whit no god results.

 

I find

code:

---

 #CNC<<MSG-ERROR(164)>>  

---

in posts. Here is one of them from posts.

 

code:

---

# Program & Sequence number format

# --------------------------------------------------------------------------

fmt 8 progno$ # Program number

fmt N 7 seqno$ # Starting Sequence No.

fmt N 7 seqinc$ # Sequence No.Increment

fmt 12 n$ # Main Program Seq No's

#CNC<<MSG-ERROR(164)>> The format statement number is not defined (default to 1)

---

thx for help :-)

 

17 Apr 2009 11:43:20 AM - <0> - Report created.

17 Apr 2009 11:43:20 AM - <2> - Initialize posting log file

17 Apr 2009 11:43:20 AM - <2> - Using MP run version 11.00 and post components version 10.00

17 Apr 2009 11:43:20 AM - <2> - Initiate opening the post processor file(s).

17 Apr 2009 11:43:20 AM - <2> - Post processor file name: D:MCAMXMILLPOSTSMPFAN.PST

17 Apr 2009 11:43:20 AM - <2> - The post processor file has been successfully opened.

17 Apr 2009 11:43:20 AM - <2> - Post version information (input):

17 Apr 2009 11:43:20 AM - <2> - UPDATEPOST Version 11. was used to modify this file.

17 Apr 2009 11:43:20 AM - <2> - The file was modified by this product on 13 Jul 05 15:05:27

17 Apr 2009 11:43:20 AM - <2> - The post was written to run with Mastercam Version 11.

17 Apr 2009 11:43:20 AM - <2> - The post product type is Mill.

17 Apr 2009 11:43:20 AM - <2> - Initialization of pre-defined post variables, strings, postblocks was successful.

17 Apr 2009 11:43:20 AM - <2> - Search for defined post variables, strings, postblocks was successful.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'err_file$' was re-initialized from 0. to 1.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'dec_seq_right$' was re-initialized from 3. to 0.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'omitseq$' was re-initialized from 1. to 0.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'sub_seq_typ$' was re-initialized from 0. to 1.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'tplanemode$' was re-initialized from 2. to 0.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'arctype$' was re-initialized from 2. to 5.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'arctypexz$' was re-initialized from 2. to 5.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'arctypeyz$' was re-initialized from 2. to 5.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'larctype$' was re-initialized from 2. to 5.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'larctypexz$' was re-initialized from 2. to 5.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'larctypeyz$' was re-initialized from 2. to 5.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'arccheck$' was re-initialized from 1. to 111.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'larccheck$' was re-initialized from 1. to 111.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'rotfeed4$' was re-initialized from 2. to 1.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'rotfeed5$' was re-initialized from 3. to 1.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'lrotfeed4$' was re-initialized from 2. to 1.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'lrotfeed5$' was re-initialized from 0. to 1.

17 Apr 2009 11:43:21 AM - <2> - CONTROL DEFINITION - - Post variable 'peckacel$' was re-initialized from 0. to 1.

17 Apr 2009 11:43:21 AM - <2> - Successful completion of posting process!

[Jim Evans from CNC Software]

Okay, This line below from your post is telling you that format statement # 12 doesn't exist so it is using FS 1.

 

code:

---

fmt    12 n$        # Main Program Seq No's

#CNC<<MSG-ERROR(164)>> The format statement number is not defined (default to 1)

---

The FS/FS2 statements in your post are used to format the numerical output of a variable, which in this case is the n$ (sequence number).

 

find a FS/FS2 statement in you post that sets up output as an integer, with no decimal, no trailing and no leading.

 

It should look somthing like the following:

code:

---

 fs2 4   1 0 1 0     #Integer, not leading 

---

Now change the FMT statement for N as shown above to the following: (the number 4 should be replaced with the number of the fs2 statement in your post that matches the fs2 statement shown above.

 

code:

---

fmt    4 n$        # Main Program Seq No's  

---

This should straighten it out for you

[arsson]

This is the FS statement in my posts

 

code:

---

# --------------------------------------------------------------------------

# Format Statements - i=incr, n=nonmodal, l=leave ldg, t=leave trlg, d=delta

# --------------------------------------------------------------------------

 

fs 1 +1.3lt

fs 2 +1.3ltn

fs 3 3 0

fs 4 2 0n

fs 5 4 0

fs 6 2 0ln

fs 7 3 0n

fs 8 4 0n

fs 9 3.3t

fs 10 1.3ltn

fs 11 +1.3ltn

#CNC<<FAIL>>fs 12 4 n

#CNC<<MSG-ERROR(101)>> The format statement processing has failed!, Inch trailing digit missing or out of range (0 to 9)

 

---

FMT statemant

 

code:

---

# --------------------------------------------------------------------------

# Program & Sequence number format

# --------------------------------------------------------------------------

fmt 8 progno$ # Program number

fmt N 7 seqno$ # Starting Sequence No.

fmt N 7 seqinc$ # Sequence No.Increment

fmt 12 n$ # Main Program Seq No's

#CNC<<MSG-ERROR(164)>> The format statement number is not defined (default to 1)

---

I think is antoher error?

What should I change?

[Jim Evans from CNC Software]

the fs 12 statement is invalid because it is missing a piece of the formating. 2 numbers are needed for the proper format, one for the integer format and one for the decimal format. The 4 is the only piece in the format making it illegal.

 

You could fix the FS statement to something like this.

 

code:

---

fs 12  4 0n  

---

Remember to remove the

code:

---

#CNC<<FAIL>> 

---

from the beginning of the fs statement so the fs lines up with the fs above it. This statement will now match fs #8 so you could also just make a change to the FMT statement as follows.

 

code:

---

fmt    8 n$        # Main Program Seq No's  

---

This should fix your problem.

[arsson]

First it not work but when i start the computer today it work fine. thanks for all help :-))