topic Re: Doosan DNM 500ii Sinumerik Post Processor in Manufacturing (CAM)

Doosan DNM 500ii Sinumerik Post Processor

mbitterwolf — Sun, 13 Dec 2020 18:37:23 GMT

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 softwareI am having some issues with the output G-Code concerning the tool Change. At the moment I get:N9 M5N10 T9 M6N11 S4000 M3with T(Position Number)What I

Re: Doosan DNM 500ii Sinumerik Post Processor

jverheyen-2 — Sat, 29 Oct 2016 10:18:31 GMT

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

Re: Doosan DNM 500ii Sinumerik Post Processor

mbitterwolf — Sun, 30 Oct 2016 09:45:54 GMT

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

Re: Doosan DNM 500ii Sinumerik Post Processor

rlysy — Mon, 31 Oct 2016 14:33:21 GMT

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