Sequence numbers at tool change

[Doug Funny]

Good Morning\Evening Gurus,

I'd like to have sequence numbers post out at every tool change and have the numbers sequence to the operation. How do I go about doing that?

 

Thanks,

Doug

[cncappsjames]

Sequence numbers at Tool Changes is handled in the Control Definition. Sequence numbers at each op would be handled in ptlchg0. Change the pbld$, n$, to pbld$, *n$,

 

Been a while since I've edited a Mastercam/IHS post. That should get you close.

[Doug Funny]

Thank you,

I'm not seeing anywhere in the control definition to set sequence numbers to tool change. Am I looking in the wrong spot?

[So not a Guru]

I added this function to a MPMaster post several years ago.

In the General output settings section:

tseqno      : 3     #Output sequence number at toolchanges when omitseq = yes
                    #0=off, 1=seq numbers match toolchange number, 2=seq numbers match tool number, 3 = Mastercam Operations Manager Operation Number

in the pprameter$ postblock add:

           if prmcode$ = 15240, opmgr_opno = rpar(sparameter$,1)      #Operation number

Turn off "Output sequence numbers in the CD:

 

[Doug Funny]

I can't find pprameter$ in my post

[So not a Guru]

8 minutes ago, Doug Funny said:

I can't find pprameter$ in my post

Whoops, it should read

pparameter$

[Doug Funny]

I was able to add the line but, when I went to post I get an error. do I need to define  opmgr_opno as a variable name?

[So not a Guru]

2 hours ago, Doug Funny said:

I was able to add the line but, when I went to post I get an error. do I need to define  opmgr_opno as a variable name?

Yes, I'm sorry. In the Misc strings section add:

opmgr_opno  : 0    #15240 - Operation number

2 hours ago, Doug Funny said:

I was able to add the line but, when I went to post I get an error. do I need to define  opmgr_opno as a variable name?

You are actually adding a string, not a variable.

1 minute ago, So not a Guru said:

You are actually adding a string, not a variable.

The added line initializes the string

[Doug Funny]

thank you, I'll add them in the morning and see how I make out

[Tim Johnson]

8 hours ago, Doug Funny said:

Good Morning\Evening Gurus,

I'd like to have sequence numbers post out at every tool change and have the numbers sequence to the operation. How do I go about doing that?

 

Thanks,

Doug

Can you show a small sample of how you want the sequence numbers to look?

[Doug Funny]

Hi Tim,

I want the N numbers to be sequential regardless of the tool number and only at the tool change. So not a Guru has gotten me to the point where I get N numbers on my tool changes but, there seems to be a bit of logic missing because they are all the same number.

 

N1 TXX M6

N2 TXX M6

N3 TXX M6

[Werktuigbouwer]

Try this:

#declaration of variables:

blockno : 0 #Mastercam operation number

 

#format statement

 

fmt  "N" 4 blockno     #Output mcam opperation no. to NC file

 

#add this starting in a first column:

pfn             #Output block numbers = mcam op number
	  blockno = opinfo(15240,0)
	  if op_id$ <> prv_op_id$ & blockno<>-99999,
	    [
	    *blockno
	    ]

#add this where the toolchange is:

pbld, *pfn, *t$, "M6",e$

 

[So not a Guru]

1 hour ago, Doug Funny said:

Hi Tim,

I want the N numbers to be sequential regardless of the tool number and only at the tool change. So not a Guru has gotten me to the point where I get N numbers on my tool changes but, there seems to be a bit of logic missing because they are all the same number.

 

N1 TXX M6

N2 TXX M6

N3 TXX M6

In the ptlchg_com postblock

After this line:

          if tseqno = 2, n$ = t$

Add this line:

      if tseqno = 3, n$ = opmgr_opno

 

[Doug Funny]

EUREKA! Thank you sir! I've been a Camworks user for most of my career and only recently started using Mastercam. This forum is so much better than any I've found for camworks. There are a lot of incredibly smart and helpful people here. More often than not, I get answers here quicker than from tech support...

[So not a Guru]

42 minutes ago, Doug Funny said:

EUREKA! Thank you sir! I've been a Camworks user for most of my career and only recently started using Mastercam. This forum is so much better than any I've found for camworks. There are a lot of incredibly smart and helpful people here. More often than not, I get answers here quicker than from tech support...

Glad I was able to help. Sorry it took so many tries, it was a long time ago that I modded that post and I'm getting senile. :)

[Doug Funny]

31 minutes ago, So not a Guru said:

Glad I was able to help. Sorry it took so many tries, it was a long time ago that I modded that post and I'm getting senile. :)

No worries. This is in no way holding me up...

[mirek1017]

I wondering ,can use sequence number to my lathe post ?

something like this 

(TOOL - 3 OFFSET - 3)
(RIGHT TURRET - 80 DEG.  INSERT - CNMG-432)
(CANED RGH OD)    -------------------------------------------------------     N1   (CANED RGH OD)
G0 T0303
M8
G97 S114 M03
G0 G54 X11.7
G0 Z.1707
G50 S1500
G96 S350

 

 

 

[crazy^millman]

1 hour ago, mirek1017 said:

I wondering ,can use sequence number to my lathe post ?

something like this 

(TOOL - 3 OFFSET - 3)
(RIGHT TURRET - 80 DEG.  INSERT - CNMG-432)
(CANED RGH OD)    -------------------------------------------------------     N1   (CANED RGH OD)
G0 T0303
M8
G97 S114 M03
G0 G54 X11.7
G0 Z.1707
G50 S1500
G96 S350

 

 

 

Sure. Need to decide how are going to sequence them and how you want the output to be controlled.

[mirek1017]

15 minutes ago, crazy^millman said:

Sure. Need to decide how are going to sequence them and how you want the output to be controlled.

I like to get N block every operation 

[crazy^millman]

Look at the old MPLMASTER post it has the process already defined in it.

[AHarrison1]

Just now, mirek1017 said:

I like to get N block every operation 

I have mine set so N# follows T#

N1 (OD 80 DEG) 
G18 G20 G40 G54 G80 G99 
G00 G53 X0. Y0. T0 
T101 
G40 G54 G80 G99 
M155 
M08 
G50 S3500 
G96 S450 M03 
G00 X2.1 Y0. Z0.01 
M88 
 
M05 
M89 
G00 G53 X0. Y0. T0 
M01 

N3 (OD 55 DEG) 
G18 G20 G40 G54 G80 G99 
G00 G53 X0. Y0. T0 
T303 
G40 G54 G80 G99 
M08 
G50 S3500 
G96 S450 M03 
G00 X1.5787 Y0. Z0.0072 
M88 
 
M05 
M89 
G00 G53 X0. Y0. T0 
M01

[mirek1017]

2 minutes ago, AHarrison1 said:

I have mine set so N# follows T#

N1 (OD 80 DEG) 
G18 G20 G40 G54 G80 G99 
G00 G53 X0. Y0. T0 
T101 
G40 G54 G80 G99 
M155 
M08 
G50 S3500 
G96 S450 M03 
G00 X2.1 Y0. Z0.01 
M88 
 
M05 
M89 
G00 G53 X0. Y0. T0 
M01 

N3 (OD 55 DEG) 
G18 G20 G40 G54 G80 G99 
G00 G53 X0. Y0. T0 
T303 
G40 G54 G80 G99 
M08 
G50 S3500 
G96 S450 M03 
G00 X1.5787 Y0. Z0.0072 
M88 
 
M05 
M89 
G00 G53 X0. Y0. T0 
M01

yes  something like this 

[mirek1017]

21 minutes ago, crazy^millman said:

Look at the old MPLMASTER post it has the process already defined in it.

so this work the same way in lathe post ?

I can find this in my lathe post 

pbld, *pfn, *t$, "M6",e$

[crazy^millman]

30 minutes ago, mirek1017 said:

so this work the same way in lathe post ?

I can find this in my lathe post 

pbld, *pfn, *t$, "M6",e$

Something has to define the pfn logic. In MPLMASTER there is this switch:

tseqno       : 2     #Output sequence number at toolchanges when omitseq = yes
                     #0=off, 1=seq numbers match toolchange number, 2=seq numbers match tool number

We then search the post to find where and how it was used:

ltlchg$          #Toolchange, lathe
. section not shown
. section not shown
. section not shown
. section not shown
      if not(synch_flg & tool_op$ = 67),     #Suppress tool output if cutoff during part xfer
        [
        if omitseq$ = 1 & tseqno > 0,
          [
          if tseqno = 2, n$ = t$
          pbld, *n$, [if home_type = -1, *sgcode], *toolno, e$
          ]
        else, pbld, n$, [if home_type = -1, *sgcode], *toolno, e$
        ]

mtlchg$          #Toolchange, mill
. section not shown
. section not shown
. section not shown
. section not shown 
      if omitseq$ = 1 & tseqno > 0,
        [
        if tseqno = 2, n$ = t$
        pbld, *n$, [if home_type = -1, *sgcode], *toolno, e$
        ]

pheader$         #Start of file
      pheader_custom
      if tseqno = 1 & omitseq$ = 1,
        [
        seqno$ = 1
        seqinc$ = 1
        n$ = seqno$
        ]

Then from there we can see what variables where defined and how we want to adapt it to the post we are using.

[mirek1017]

4 minutes ago, crazy^millman said:

Something has to define the pfn logic. In MPLMASTER there is this switch:

tseqno       : 2     #Output sequence number at toolchanges when omitseq = yes
                     #0=off, 1=seq numbers match toolchange number, 2=seq numbers match tool number

We then search the post to find where and how it was used:

ltlchg$          #Toolchange, lathe
. section not shown
. section not shown
. section not shown
. section not shown
      if not(synch_flg & tool_op$ = 67),     #Suppress tool output if cutoff during part xfer
        [
        if omitseq$ = 1 & tseqno > 0,
          [
          if tseqno = 2, n$ = t$
          pbld, *n$, [if home_type = -1, *sgcode], *toolno, e$
          ]
        else, pbld, n$, [if home_type = -1, *sgcode], *toolno, e$
        ]

mtlchg$          #Toolchange, mill
. section not shown
. section not shown
. section not shown
. section not shown 
      if omitseq$ = 1 & tseqno > 0,
        [
        if tseqno = 2, n$ = t$
        pbld, *n$, [if home_type = -1, *sgcode], *toolno, e$
        ]

pheader$         #Start of file
      pheader_custom
      if tseqno = 1 & omitseq$ = 1,
        [
        seqno$ = 1
        seqinc$ = 1
        n$ = seqno$
        ]

Then from there we can see what variables where defined and how we want to adapt it to the post we are using.

I hope  I can get only .00001%  your  knowledge