post proccesor

[corrie]

I,m using cncpro to run my machine,and need a post to generate code using photov carve,tried the mach 2/3 inch.txt but get funny things happening when I run the code .I edited the code but ended up where the machine left home position ,went + x to the limit of the code then returned to 0,0 then went back to the x limit and thought that was the start point.re-wrote the code and same results.Wierd.Which post should I use that is available with Photo-v-carve to save my files to .Hope this makes sence,cheers and thanks in advance.

[DayneInfo]

You may want to post your question here also. http://vectric.com/forum/index.php Lots of help available

Dwayne

[Switcher]

Originally Posted by corrie I,m using cncpro to run my machine,and need a post to generate code using photov carve,tried the mach 2/3 inch.txt but get funny things happening when I run the code .I edited the code but ended up where the machine left home position ,went + x to the limit of the code then returned to 0,0 then went back to the x limit and thought that was the start point.re-wrote the code and same results.Wierd.Which post should I use that is available with Photo-v-carve to save my files to .Hope this makes sence,cheers and thanks in advance.

Show us the post you have (.txt file).

Might help us, help you.


.

[corrie]

I deleted the original .txt,but because I have cut3d as well I cut and pasted one of the posts from cut3d and imported it into photo v carve.I used ez router.txt from there and it seems fine.I,ll do some cuting tommorow and see what comes up.thanks for the responce all.

[Switcher]

I can show you how to make a custom post in "Vcarve", from your "Cut3D post". So you'll never have to copy & past again.

And to delete all the other post you'll prob. never need, so they don't show up in "Vcarve"






.

[corrie]

Hey Switcher and to all a Happy New Year.I just found that saving a file in photovcarve confused me for a moment,not sure which post-p to actualy use.Like I said before the closest looking match was the Mach2/3inch.txt ,so I thaought.I didn,t need any lines for tool change or spindle or coolant.There is still lots I need to learn,but hey I,m learning.As many of you know CNC-PRO is a DOSbased controler,I,m thinking of going to a windows based one in the spring,we,ll see.Ok Switcher show me the money,L.O.L.....cheers.

[Switcher]

This is how to create a new custom post for "Vcarve".

Note: Windows XP, VCarve Pro 3.0 Trial Edition

1) Open the the file "VCarve Pro 3.0 Trial Edition", my default location when I downloaded from the Vcarve website was "C:\Program Files\VCarve Pro 3.0 Trial Edition"

2) Copy & Paste a copy of the "PostP" file (you can paste it into the "VCarve Pro 3.0 Trial Edition" file, the program will ignore it) we need to have a backup just incase. So we should now have a new file called "Copy of PostP". Just remember that the program is always looking for the "PostP" file-name, so don't re-name that file.

3) Open the file "PostP"

4) I'm working with the "Mach2_3_inch" post (That's all I want to show up when I run the actual Vcarve program, I will never need all the other post because my cnc machine setup will remain the same), so delete everything except the "Mach2_3_inch" post (make sure you did the step that created a backup of all the post).

5) Open the "Mach2_3_inch" post, with Windows Notepad, It should look like the below file:

+================================================ + + Mach2/3 - Vectric machine output configuration file + +================================================ + + History + + Who When What + ======== ========== =========================== + Tony 15/11/2005 Written +================================================ POST_NAME = "Mach2/3 (inch) (*.txt)" FILE_EXTENSION = "txt" UNITS = "inches" +------------------------------------------------ + Line terminating characters +------------------------------------------------ LINE_ENDING = "[13][10]" +------------------------------------------------ + Block numbering +------------------------------------------------ LINE_NUMBER_START = 0 LINE_NUMBER_INCREMENT = 10 LINE_NUMBER_MAXIMUM = 999999 +================================================ + + Formating for variables + +================================================ VAR LINE_NUMBER = [N|A|N|1.0] VAR SPINDLE_SPEED = [S|A|S|1.0] VAR FEED_RATE = [F|C|F|1.1] VAR X_POSITION = [X|C|X|1.4] VAR Y_POSITION = [Y|C|Y|1.4] VAR Z_POSITION = [Z|C|Z|1.4] VAR X_HOME_POSITION = [XH|A|X|1.4] VAR Y_HOME_POSITION = [YH|A|Y|1.4] VAR Z_HOME_POSITION = [ZH|A|Z|1.4] +================================================ + + Block definitions for toolpath output + +================================================ +--------------------------------------------------- + Commands output at the start of the file +--------------------------------------------------- begin HEADER "( [TOOLPATH_NAME] )" "( Mach2/3 Postprocessor )" "[N]G00G20G17G90G40G49G80" "[N]G70" "[N]T[T]M06" "[N]G00G43[ZH]H[T]" "[N][S]M03" "[N]G94" "[N][XH][YH][F]" +--------------------------------------------------- + Commands output for rapid moves +--------------------------------------------------- begin RAPID_MOVE "[N]G00[X][Y][Z]" +--------------------------------------------------- + Commands output for the first feed rate move +--------------------------------------------------- begin FIRST_FEED_MOVE "[N]G01[X][Y][Z][F]" +--------------------------------------------------- + Commands output for feed rate moves +--------------------------------------------------- begin FEED_MOVE "[N][X][Y][Z]" +--------------------------------------------------- + Commands output at the end of the file +--------------------------------------------------- begin FOOTER "[N]G00[ZH]" "[N]G00[XH][YH]" "[N]M09" "[N]M30" %

6) Everything in red is all info that theVcarve program needs to add a Header & Footer to the g-code it creates, you can edit this (Header & Footer) to your own custom needs. You can change ( POST_NAME = "Mach2/3 (inch) (*.txt)" ) So it reads a custom name in the dropdown list when you save the g-code in the actual Vcarve program, like "Switchers New Post (*.txt)" (see screenshot).

7) You could edit LINE_NUMBER_INCREMENT = 10 .

8) I think, the rest of the code explains itself well enough.

9) I can't say it enough, Backup everything you do!

10) This will allow you edit Header & Footer.



.

[corrie]

Thanks Switcher for the help I,ll take a run at doing that but does it mater if I don,t have V-carve.Can I do it from Cut3D.Maybe a silly ? but had to ask,cheers.

[Switcher]

Originally Posted by corrie Thanks Switcher for the help I,ll take a run at doing that but does it mater if I don,t have V-carve.Can I do it from Cut3D.Maybe a silly ? but had to ask,cheers.

Yep, same thing, file name etc...

I just checked, I have both.

.