Have the "Post CD" but where to start??

[Dustin S.]

After researching on here and fiddling with the posts myself I called my reseller and got a copy of the "POST cd" but its all just kinda thrown on there not sure where to start... I can list whats on the CD but ill start by asking for a suggestion?

 

Hand outs folder (printed these out)

Control Def. review Power point (watched it)

Machine Def. review power point (watched it)

5 axis generic post power point (don't need to watch)

Examples folder

MD CD FAQ folder

MD CD Over View folder

Modules folder

Basic Post 2007 power point (watched it)

Mcamx_post_parameter_reference PDF

MC Definitions PDF

whats new x2 post PDF

X2_post_installation_setup .exe

 

let me know maybe i'm missing something but i watched the basic Post 2007 and it didn't go sequentially I have a basic understanding but like right now I want to edit start-up codes and NO CLUE where to start

[Guest]

quote:

---

right now I want to edit start-up codes and NO CLUE where to start

---

Well, you need to turn on the debugger and figure our what section of the post is actually outputting the section that you want to change.

[Mick]

What post CD is this? I thought the most recent Post CD was for V9?

[Guest]

it is Mick

[M_CODE1]

John,

 

How do you turn on the "debugger"???

 

Thanks

[Nils N]

It's in the Chook folder, ALt>C will bring up the chooks then look for UdatePost.dll you can also find some help in the help section (Update Post dialog box)

[Guest]

quote:

---

How do you turn on the "debugger"???

---

Go into your control def >> nc output >> click on "enable post file debug information"

 

It's near the upper right corner of the window

 

hth

[Colin Gilchrist]

By "start up codes" I'm assuming you mean that you want to change the format of the saftey line output at the NC file header.

 

These codes are generally output by the psof (start of file) post block. In addition to psof, some of the output might be included in the toolchange output blocks, which is usually ptlchng$ or ptlchng0$.

 

Ptlchng$ is the "standard" tool change post block (when a tool is actually changed) and ptlchng0$ is the "null" toolchange, when the same tool is used in multiple toolpath operations in Mastercam.

 

Why don't you post up a sample of the NC output and let us know what you what to change. Then we can help you from there.

 

HTH,

[Dustin S.]

You are all correct... I knew about the debugger but wasn't sure how it worked Im gonna try to do a little more myself but Ill post it if I can't figure it out. The little bit of information here helped me get out of my rut!

 

Thank you to everyone

[Dustin S.]

Well that was fast :-p im tryingto get rid of all the tool information after 1/4 3-fl iscar and the / g91...

/g28....

/g92....

 

thought that was debug related information ?! but it doesn't turn off...

 

 

( T1 | 1/4 3-FL ISCAR | H1 | D1 | WEAR COMP | TOOL DIA. - .25 ) pwrtt$ ptooltable 68.

( T2 | 1/8SHANK .125DIA .0313CR E.M. | H2 | D2 | WEAR COMP | TOOL DIA. - .125 ) pwrtt$ ptooltable 68.

/ G91 G28 Z0. psof$ p__4:830 70.

/ G28 X0. Y0. psof$ p__4:830 70.

/ G92 X10. Y10. Z10. psof$ p__4:830 70.

( 1/4 3-FL ISCAR | TOOL - 1 | DIA. OFF. - 1 | LEN. - 1 | TOOL DIA. - .25 ) psof$ ptoolcomment 70.

psof$ psof$ 70.

T1 M6 psof$ psof$ 70.

G0 G40 G43 G90 psof$ psof$ 70.

X.1536 Y-.325 A0. Z2. H1 M3 S4000 psof$ psof$ 70.

Z.1 pzrapid$ prapidout 72.

G1 Z-.144 F50. plin$ plinout 74.

G41 D1 Y-.245 F8. plin$ plinout 76.

G3 X.0786 Y-.17 R.075 pcir$ pcirout 78.

G1 X-.0786 plin$ plinout 80.

G2 X-.2308 Y-.0441 R.155 pcir$ pcirout 82.

X.235 Y0. R.235 pcir$ pcirout 84.

X.2308 Y-.0441 R.235 pcir$ pcirout 86.

X.0786 Y-.17 R.155 pcir$ pcirout 88.

G3 X.0036 Y-.245 R.075 pcir$ pcirout 90.

G1 G40 Y-.325 plin$ plinout 92.

Z.1 F500. plin$ plinout 96.

G0 Z2. pzrapid$ prapidout 98.

G91 G28 Z0. ptlchg1002$ p__9:934 164.

M01 ptlchg$ ptlchg$ 166.

[Dustin S.]

Not sure I want to post my whole machine post here so let me know what you might need to help me out...

 

Thanks again

[bigjohn]

Make a couple of copies of your post before you edit anything.

Try typing "#" before the line you don't want to output.

[Dustin S.]

the debugging option helped ALOT and am using # to kill code i don't want... worken great and back-up saving every time I hit a benchmark

 

Still can't figure out how to kill the tool offset # diameter offset# workoffset# and such as listed above

[Kyle Waters]

Dustin,

 

It is in the ptoolcomment section of your post..

[Dustin S.]

I got it all figured out now... I did the ole' trial and error method I can now take stuff out of a post using # < that wonderful character!

 

I used the debugging feature to find the sections in the post I wanted to edit made one change at a time posting results till I got what I wanted...

 

This topic is wrapped up

 

Thanks for the help