Are there any tutorials online that will walk someone through their first post edit?
Basically I want to add some remark fields to the top of the NC file with customer info, part name, dwg #, mc9 file name and date that I can fill in by hand as required. I also have to hand edit out A0. and don't want my table to home at every tool change so G28 X0.Y0.A0. has to go.
I'd also like to add an automatic G0 Z2.5 M09; X0. Y2.0 at the end of the program before homing the spindle and rewinding the program. Most of the parts we make allow for this table travel with my set ups and it would be very convienent if the post would add this for me. As it is now I have use the replace function in the simco editor and then hand edit the rest in. I'm using the generic mpfan post for Haas TM-1s. TIA
Scott

Put it in the Haas and use the Haas editor. You should be able to do all your changes using the find/replace function. For your identification stuff at the top you can create a little program that has all the fields blank. You call up this program, enter your stuff in all the fields, select the whole program as a block, copy it to the clipboard and then paste it from the clipboard into the top of your program.

Do you want to buy one that already has all that in it?

Mike Mattera

Are there any tutorials online that will walk someone through their first post edit?
Basically I want to add some remark fields to the top of the NC file with customer info, part name, dwg #, mc9 file name and date that I can fill in by hand as required. I also have to hand edit out A0. and don't want my table to home at every tool change so G28 X0.Y0.A0. has to go.
I'd also like to add an automatic G0 Z2.5 M09; X0. Y2.0 at the end of the program before homing the spindle and rewinding the program. Most of the parts we make allow for this table travel with my set ups and it would be very convienent if the post would add this for me. As it is now I have use the replace function in the simco editor and then hand edit the rest in. I'm using the generic mpfan post for Haas TM-1s. TIA
Scott

I'm very new to MC so forgive me if I screw something up. You can edit a post processor in the Posts Folder.

Main Menu
File
Edit
PST.

Your Post Processor list will come up and you can edit the HAAS Posting by double clicking on it. This opens a new window showing the entire Post Processor Script. There are plenty of directions in MC's main folder on your "C/:" drive.

A lot of the options are self explanitory and others are actual VB Scripts.
Look around a little and see what you can find.

This one is from MC8 Level 1 I believe. I have no idea if it has been edited so don't use it for posting g-code that your going to run. Your better off using this to play with and to get used to the MC Posting Language.

:cheers:

I'll see if I can help. I made similar changes to my toolchange, removing A's, etc.
Open the post in notepad. Look for something like this:

# ------------------------------------------------------------------------
# Start of File and Toolchange Setup
# -----------------------------------------------------------------------

Their are several subheadings under this, like "#Start of file for non-zero tool number" and "#Tool change".
Under a few of the subheadings is the line
"pfbld, n$, *sg28ref, "X0.", "Y0.", e$"
what I would do at this point is make a change and try the post. I'm not sure if you would need to make the change under each subheading or not, experiment. For example if you just wanted to home the z axis, change the line to:
pfbld, n$, *sg28ref, "Z0.", e$

Adding the lines to the top of the program is going to take much more thought. I need to do something similar, though, so if I get around to it I will update.

Hope this helps,

Joe

edit:
BACKUP POST FIRST!!!
end edit.

To turn off the A axis, go to the bottom of the post and look for question 164 and set it to "n" for no output.

General post editing information.
http://www.mmattera.com/
got to Technology - Mastercam Stuff and then "How To Edit A Post".

Mike Mattera

Put it in the Haas and use the Haas editor. You should be able to do all your changes using the find/replace function. For your identification stuff at the top you can create a little program that has all the fields blank. You call up this program, enter your stuff in all the fields, select the whole program as a block, copy it to the clipboard and then paste it from the clipboard into the top of your program.

I appreciate the advice but am not sure if that would be ideal for our circumstances. I frequently use find and replace for fine tuning programs but want the field for archival purposes on my laptop. Since I will be burning them on cd from my laptop I need these on the file at generation, not at the controller. It is my practice to take notes on changes I make to fine tune a program at the controller and make these same changes in the design file and then post the file again with the changes.

The machinist before me left under bad circumstances and a lot of blueprints are missing. The owners think he took them with himand as a result when hired I was told explicitly that all files and blueprints were to be keep filed, provided with a new filing cabinet, folders, CDs and floppies with sleeves for both. Since our main customers track who has what proprietary blueprints they are touchy about our asking for new prints when they show we signed for a copy less than a year ago. It looks unprofessional and the owner has set policy and I need to follow it.


Thanks
Scott

Do you want to buy one that already has all that in it?

Mike Mattera

Possibly, send me a price as a private message. I'm not sure what the rules are about commercial discussion in this forum so I don't want to inadvertantly violate the rules.
Personally I'm kind of hands on and am always trying to learn more about how things work, ecspecially as a new graduate starting a second career, so I'd like to do it myself, but for a reasonable price it would be worth having an edited post specific to our machines.

I'll see if I can help. I made similar changes to my toolchange, removing A's, etc.
Open the post in notepad. Look for something like this...

Thanks, to you, Mike and eveyone else. I've looked around in the pst file but haven't tried to change anything, only looked around. I'll try it and then carefully read my resulting nc files.

Love the sig line btw
Scott

Possibly, send me a price as a private message. I'm not sure what the rules are about commercial discussion in this forum so I don't want to inadvertantly violate the rules.
Personally I'm kind of hands on and am always trying to learn more about how things work, ecspecially as a new graduate starting a second career, so I'd like to do it myself, but for a reasonable price it would be worth having an edited post specific to our machines.

Scot,

You can copy a post to Modify leaving the original alone and unaltered. That is the safest way I know of. I am totally new to MC and everything about it and found that most of the standard guidelines of other softwares apply to MC as well. What I am doing is modifying a Copied Post Processor and posting G-Code with it to see what changes in the end result. When making changes keep in mind to change one thing at a time taking notes of what was changed. Also keep a Text Log to reference while editing a post (PST. File).

Those books and videos of Mikes look very good. I may purchase them myself.

I'm very new to MC so forgive me if I screw something up. You can edit a post processor in the Posts Folder.

Main Menu
File
Edit
PST.


Holy cow! A years old post but you just answered a question I couldn't get straight whether I asked my VAR or bugging the guys at the MC booth at Westec. A hundred thanks!

I kept getting told that I needed to do it all through the machine and control defs.

I'm finally going to get that post cleaned up (2.5 years later).

Well Hotkey if you had gone over to the emastercam forum you would have had that answered in about 15 minutes.

http://www.emastercam.com/cgi-bin/ultimatebb.cgi

Shotout, how about this layout for you.
%
O0001 (T REV: )
(T )
(MACHINE TOOL : HAAS VMC )
(DATE -06-12-07 )
(TIME -19:08 )
(*)
(MATERIAL: )
(STOCK SIZE: X = 0. Y = 0. Z = 0. )
(HOME POSTION COORIDNATES ARE THE FOLLOWING)
(X= )
(Y= )
(Z= TOP OF PART)
(*)
( TOOL - 1 DIA. - .3125 5/16 FLAT ENDMILL )
( TOOL - 2 DIA. - .031 #68 DRILL )
(*)
(USING FIXTURE OFFSETS: G54 )
(*)
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T1 M6 ( TOOL - 1 DIA. - .3125 5/16 FLAT ENDMILL )
N106 G0 G90 G54 X.2281 Y-1.9064 S4889 M3
N108 G43 H1 Z.25
N110 Z.1
N112 G1 Z0. F6.4
N114 Y-1.5939 F24.2
N116 G3 X-.0844 Y-1.2814 I-.3125
N118 G1 X-2.3878
N120 G2 X-2.5441 Y-1.1252 J.1562
N122 G1 Y1.419
N124 G2 X-2.3878 Y1.5752 I.1563
N126 G1 X2.2191
N128 G2 X2.3753 Y1.419 J-.1562
N130 G1 Y-1.1252
N132 G2 X2.2191 Y-1.2814 I-.1562
N134 G1 X-.0844
N136 G3 X-.3969 Y-1.5939 J-.3125
N138 G1 Y-1.9064
N140 Z.1 F6.4
N142 G0 Z.25 M9
N144 T2 M6 ( TOOL - 2 DIA. - .031 #68 DRILL )
N146 G0 G90 G54 X-1.844 Y1.0314 S5000 M3
N148 G43 H2 Z.1
N150 G99 G81 Z0. R.1 F1.4
N152 X-1.869 Y-.5251
N154 X1.4252 Y-.6438
N156 X1.5815 Y.7064
N158 G80 M9
N160 G0 Z2.5 X0. Y2.0
N162 G91 G28 Z0.
N164 G28 Y0.
N166 M30
%

if you use the stock setup it will put that info in the stcok location. and it will tell you all the offsets and what they are.I add the little info you asked for at the end so it posts out.
Would this be what you want?

cadcam

I appreciate it but that post was from Oct 06 and was revived. I had edited the post but since we have upgraded and have machine specific posts we purchased from our reseller. Thank you though for taking the time to answer.