TOOL LIST

[MCFELIX]

HI EVERYBODY, I HAVE ONE QUESTION ,HOW OBTAIN TOOL LIST AT BEGINNING OF MY PROGRAM,HOW I CAN CHANGE IN THE POST (MPFAN)THANKS EVERYBODY

[Michael Reynolds]

Hi Felix!

Welcome to the forum! Anyway, if you use the mpmasterpost, your tool list will come up at the beginning of your program. You can download mp master post from the "posts" page at the top of this page.

BTW, if you type in caps, people think you're shouting at them.

hope this helps!!

Mike R.

[ 12-17-2001: Message edited by: Michael Reynolds ]

[Roger Martin from CNC Software]

To get the MPFAN.PST (from the v8.1.1 CD) to output a list of the tools

used in the program to output at the start of the NC file ->

First, you must tell the PST to do a pre-scan of the NCI file.

Add this varaible to the MPFAN.PST ->>

tooltable : 1 #Do a pre-scan of the NCI (calls postblock 'PWRTT')

Now you need to add the PWRTT postblock that will be called because

of the 'tooltable' setting. We will just have this call the PTOOLCOMMENT

postblock that already exists in the PST.

pwrtt # Called at each toolchange (and NULL toolchange) in the program

if t > 0, ptoolcomment # Only do if T > 0 (at a real toolchange)

------------------------------------------------------------------------------------------------------------

Note that the tool list will output PRIOR to the '%' at the start of the NC file.

If you wish to reposition the tool list so that it outputs after the initial NC startup

blocks, you would relocate the startup blocks. Move them from PSOF and

place them into the PHEADER postblock.

pheader #Call before start of file

if met_tool = one, #Metric constants and variable adjustments

[

ltol = ltol_m

vtol = vtol_m

maxfeedpm = maxfeedpm_m

]

# Start of NC file.... following lines relocated from PSOF postblock ->>

"%", e

*progno, e

"(PROGRAM NAME - ", progname, ")", e

"(DATE=DD-MM-YY - ", date, " TIME=HH:MM - ", time, ")", e

The result in output such as ->

%

O1234

(PROGRAM NAME - MTEST)

(DATE=DD-MM-YY - 17-12-01 TIME=HH:MM - 10:27)

(1/4 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .25)

(5/16 FLAT ENDMILL TOOL - 4 DIA. OFF. - 4 LEN. - 4 DIA. - .3125)

(3/8 DRILL TOOL - 3 DIA. OFF. - 3 LEN. - 3 DIA. - .375)

(1/4 CENTERDRILL TOOL - 5 DIA. OFF. - 5 LEN. - 5 DIA. - .25)

N100G20

N102G0G17G40G49G80G90

[Trevor Bailey]

WOW!!! Now that is an explaination. Glad to see we have a lot of "post" guys in here now.

[MCFELIX]

hey mychael ,what is the diference betwen mpfan and mpmaster, i can used mpmaster for diferents controls

[Allan Brown]

Mpmaster is my own 'child' of Mpfan. It has some additions to tackle commonly requested post functionality - like a tool table for instance.

We use it here at In-House to as a starting point for 3/4-Axis machines with somewhat standard G-Code.

Mpfan is CNC Software's flagship post, and certainly can be modified to cover more than just Fanuc controls. It's been my experience that starting with a solid post and modifying it to suit saves time and headaches in the long run.

[Michael Reynolds]

Hi Felix! Looks like Dave beet me to the punch. MPmasterpost is an awsome post, though.

Ta,

Mike R.

[Guest CNC Apps Guy 1]

I've found I can get ALOT more accomplished starting from MPFAN or MPMASTER. Both are excellent places to start IMHO. They have most all the logic you'd even need for 3-4 axis machine. They don't have everything but, they certainly come close.

JM2C

[Michael Reynolds]

I agree, I started with mp ez post for use on simple 3 axis generic fanuc controllers, and found it to be FLAWLESS. Then when using our 4th axis horizontal fanuc, MPfanpost worked good with a few modifications. THEN, I started using MP masterpost for the 4th axis stuff (and sub programming), and will not go back (unless I'm programming for a simple 3 axis VMC.

Mike R.