Skip to main content
M
mbitterwolf1-Visitor
1-Visitor
October 28, 2016
Question

Doosan DNM 500ii Sinumerik Post Processor

  • October 28, 2016
  • 1 reply
  • 3335 views

Hi there,

I am currently setting up a 3-Axis DNM Doosan 500ii with a Siemens Sinumerik 828D Control and Creo 3.0 as the CAM software

I am having some issues with the output G-Code concerning the tool Change.

At the moment I get:

N9 M5

N10 T9 M6

N11 S4000 M3

with T(Position Number)

What I Need is:

N9 M5

N10 T="Tool Name" M6

N11 S4000 M3

is there anyone that could help me?

Thank you!


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

1 reply

J
jverheyen-21-Visitor
1-Visitor
October 29, 2016

Hello,

As an instant solution you can easily substitute T9 by "ENDMILL DIA 10" by example.

On a longer term you have to correct your postprocessor.

We did it for our own DMG machining centre with Siemens 840Dsl.

If you send me a CL file, I can postprocess it for you to show you that it works.

Best regards,

Jef Verheyen,

KU Leuven

Faculty of Industrial Engineering

Campus De Nayer

2860 Sint-Katelijne-Waver

Belgium

M
mbitterwolf1-VisitorAuthor
1-Visitor
October 30, 2016

Thank you for your fast reply!

With the instant solution I already had my code running but because I am working as a student for a chair of my univerisity they want me to correct the postprocessor.

I tried putting in some fil data:

CIMFIL/ON,PPRINT

$$ Macro to store the tool name in a variable

$$ to re-issue with the tool change

TXT=TEXT/CLW $$ Text of message

TEST=TEXT/'TOOL NAME' $$ Text to test for

OKCOM=INDXF(TXT,TEST)

IF (OKCOM.NE.0) THEN

  $$ This is a tool comment

  MESS=TEXT/OMIT,TXT,1 $$ Omit trailing blank

  COL=TEXT/':'

  COLPOS=INDXF(MESS,COL) $$ position of : in MESS

  LEN=CANF(MESS,1) $$ number of char in MESS

  NMESS=TEXT/RANGE,MESS,COLPOS+1,LEN $$ Extract from : to end

ELSE

  DMY=POSTF(13) $$ Process

ENDIF

CIMFIL/OFF

CIMFIL/ON,LOADTL

IF (OKCOM.EQ.0) THEN

  DMY=POSTF(13) $$ Process

ELSE

  $$ Tool name programmed

  XX=POSTF(2,1,1867,1) $$ no tape output

  DMY=POSTF(13) $$ process tool change

  TNUM=POSTF(7,4) $$ Tool number

  XX=POSTF(2,1,1867,0) $$ re-activate tape output\

  INSERT/'T',TNUM,'M6(',NMESS,')$'

ENDIF

CIMFIL/OFF

But it had some issues with this code and output an error.

Maybe someone can spot my mistake or point me in the right direction?

Kind regards

R
rlysy10-Marble
10-Marble
October 31, 2016

Hi,

I have modified your macros little bit.

Notice that Cimfil MACHIN macro was added too.

CIMFIL/ON,PPRINT
$$ Macro to store the tool name in a variable
$$ to re-issue with the tool change

TXT=TEXT/CLW $$ Text of message
TEST=TEXT/'TOOL NAME' $$ Text to test for
OKCOM=INDXF(TXT,TEST)

IF (OKCOM.NE.0) THEN
  $$ This is a tool comment
  MESS=TEXT/OMIT,TXT,1 $$ Omit trailing blank
  COL=TEXT/':'
  COLPOS=INDXF(MESS,COL) $$ position of : in MESS
  LEN=CANF(MESS,1) $$ number of char in MESS
  NMESS=TEXT/RANGE,MESS,COLPOS+1,LEN $$ Extract from : to end
  NMESS=TEXT/OMIT,NMESS,3     $$ Omit all spaces
ELSE
  DMY=POSTF(13) $$ Process
ENDIF

CIMFIL/OFF

CIMFIL/ON,LOADTL

IF (OKCOM.EQ.0) THEN
  DMY=POSTF(13) $$ Process
ELSE
  $$ Tool name programmed
  XX=POSTF(2,1,1867,1) $$ no tape output
  DMY=POSTF(13) $$ process tool change
  TNUM=POSTF(7,4) $$ Tool number
  XX=POSTF(2,1,1867,0) $$ re-activate tape output\
$$  INSERT/'T',TNUM,'M6(',NMESS,')$'
  INSERT/' T="',NMESS,'" M6$'
  OKCOM=0    $$ Initialization
ENDIF

CIMFIL/OFF

CIMFIL/ON,MACHIN
   DMY=POSTF(13) $$ Process
   OKCOM=0   $$ Initialization
CIMFIL/OFF

Now, when the tool name is outputed via PPRINT, tool record will be in format: T="TOOL_NAME" M6

When the tool name is NOT outputed via PPRINT, tool record will be in format: T=TOOL_NUMBER M6

Regards

    Terms & ConditionsCookie settingsAccessibility statement