add ptoolcomment to post

[connormac]

When I had some problems ya'll suggested that I run MPfan to see if it was a post problem or what. I noticed that MPfan had ptoolcomment that put in some cool stuff. Question is is it worth having. Do any of you use it. And how big of a pain would it be to get in my post's. I just can't leave stuff alone

 

Thanks for your input

[Guest CNC Apps Guy 1]

Not a big PITA at all. Well worth it if you ask me. You can be as detailed as you want to be or just use a simple desc.

 

Here's my snippet...

 

Enjoy,

 

code:

---

ptoolcomment    #Comment for tool

tnote = t

toffnote = tloffno

tlngnote = tlngno

tldianote = tldia

"(", pstrtool, *tnote, *toffnote, *tlngnote, *tldianote, ")", e

---

HTH

[crazy^millman]

Have you loooked at MPMASTER availbe off of this web site it pretty much is the porshe of post you can get for free in my mind. I use it for just about every machine we have or big parts of it.

 

HTH

[connormac]

James,

Do I just add what you put or do I have to put stuff in other parts of post??

 

Yes Crazy I will try MPMASTER.

 

Thanks for input

[Steve Biehl - Cimquest Inc]

CM,

in the psof and ptlchg sections, you would put a call to ptoolcomment.

You will also need the format statements for, tnote, toffnote, tlngnote, and tldianote. Search the mpfan post for these and cut and paste into your post.

 

Always have a backup before editting posts!!!

[connormac]

Thanks Steve James & Crazy,

 

That worked great. Now I want to put in the min & max on Z depths.

 

 

Thanks

[Roger Martin from CNC Software]

From Topic: Capture a Value

 

How you do it depends on what data you are trying to capture. Some data can be collected using the PWRTT postblock (which is activated using the TOOLTABLE variable set to '1' or '3')

For example you can collect x_min, y_min and z_min using this method, which is how the MILL.SET does it.

[Don S at Barefoot CNC South]

Hi

T00L TABLE AT THE TOP OF PROGRAMS

code:

 

fmt 12 day

fmt 12 year2

 

year2 = year + 2000

 

 

fmt TOOL- 3 tnote # Note format

 

 

 

then . . .

code:

 

pheader # file name

"%"

progno, " (", progname, ")"

"( ", mon, " ", day, " ", year2, ")"

"(PROGRAM NO.", *progno, ")"

"(TOOLS)

 

 

Along with this:

code:

 

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

# Tooltable Output

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

 

pwrtt # Write tool table, scans entire file, null tools are negative

tnote = t

strtool = ucase(strtool)

if t >= 0, "(", tnote, "-", strtool, ")"

if t >= 0, tcnt = tcnt + 1

 

 

 

 

Set the variable tooltable to yes (1) or add to variable if not there to enable the execution of pwrtt.

Here are two lines of code that will help.

code:

 

 

bldnxtool : yes # Build next tool table

 

tooltable : 1 # Read for tool table and pwrtt

 

 

tcnt : 0 # Count the number of tool changes

 

Just to add soemthing to this guys if you want a little more information is over a netwrok you can add this to the post also:

code:

 

"(MC9 FILE - ", smcpath, smcname, smcext, ")", e

"(PROGRAM LOCATION - ", spathnc, snamenc, sextnc, ")", e

 

 

This tells you where on the network the files was placed if doing DNC and also tells you where the MC9 file is also.

 

 

Results:

 

%

O1001 (204014_23300_SM1 )

( Apr 1 2004 )

(PROGRAM NO. O1001 )

(TOOLS)

( TOOL-1 - 5/8" ---GT SPOT DRILL )

( TOOL-2 - 5/16 ---GT DRILL )

( TOOL-3 - 11/32 FULLERTON 30812 BALL EM )

( TOOL-4 - 13/64 ---GT DRILL )

( TOOL-5 - 9/64 ---GT DRILL )

( TOOL-6 - 3/32 FULLERTON 30609 CEM 4-FLUTES )

( TOOL-7 - OSG HYPRO 45 DEG CHAMFER TOOL )

( TOOL-8 - 1/4-20 TAP )

[Don S at Barefoot CNC South]

Hi

Also could add

 

Example:

%

:0000 (258A4720NC)

(HOVIS- MACHINE CNC: HAAS VF-8/50 )

(MATERIAL -STEEL inch - 4140 - 400 BHN)

(POST - MPHAAS_VF8_3X_POST)

(DATE: 16-08-04)

(PROGRAM GENNERATED IN MASTERCAM vers_no 9.)

(PROGRAMER: DON S)

(STOCK SIZE: X20. Y20. Z.1 )

(STOCK ORIGIN: X0. Y0. Z0. At Center, Z at Top)

code:

 

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

#Select stock orientation note

stk0 "At Center, Z at Top"

stk1 "Upper Left corner, Z at Top"

stk2 "Upper Right corner, Z at Top"

stk3 "Lower Right corner, Z at Top"

stk4 "Lower Left corner, Z at Top"

stk5 "Upper Left corner, Z at Bottom"

stk6 "Upper Right corner, Z at Bottom"

stk7 "Lower Right corner, Z at Bottom"

stk8 "Lower Left corner, Z at Bottom"

stknote

 

fstrsel stk0 stck_crnr stknote

 

fmt 12 day

fmt 12 year2

 

year2 = year + 2000

 

 

fmt TOOL- 3 tnote # Note format

 

fmt X 11 stck_ht # X - Stock Height

fmt Y 11 stck_wdth # Y - Stock Width

fmt Z 11 stck_thck # Z - Stock Thickness

fmt X 2 stck_x # X origin of block

fmt Y 2 stck_y # Y origin of block

fmt Z 2 stck_z # Z origin of block

fmt 2 stck_crnr # Origin corner of stock

 

 

#at pheader

"(MATERIAL -", *stck_matl, ")", e

"(POST - ", spostname, ")", e

"(DATE: ", date,")", e

"(PROGRAM GENNERATED IN MASTERCAM ", *vers_no ,")", e

"(PROGRAMER: ", perg1, sperg1,")", e

"(STOCK SIZE: ", *stck_ht, " ", *stck_wdth, " ", *stck_thck, " ", ")", e

"(STOCK ORIGIN: ", *stck_x, " ", *stck_y, " ", *stck_z, " ", *stknote, ")", e

 

 

#Added

pstock_info # output stock information if requested

 

 

#End of added

[Guest CNC Apps Guy 1]

I always start with MPMaster too. It is THE most dialed post youcan get for free. Lots of cool features.

[connormac]

Thanks All,

 

I downloaded MPMaster and will try it. Will just have to put in all the stuff I created in my posts.

 

Thanks again