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.

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

Dwayne

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. :)


.

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.

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"






.

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.

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.



.

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.

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.

.