V2 Vectric Post Processor in Vectric 11

As of 11/15/21, Vectric (Vcarve/aspire/cut2d) has updated it post processor to V2. This combines cnc and laser operations into one post processor.
In vectric 11, you’ll need to click the cloud logo in the upper right hand side to update the database to find the new post processor. All Onefinity machines use the same one, even though the configuration wizard makes you choose your specific model.
Please report any issues with this post processor to support@onefinitycnc.com.

4 Likes

Wow. That was quick and easy!

1 Like

let us know how they work out for you

What are the measurements for the Journeymen X-50 Width and Height?

I think the height is same 32.125.

So does this eliminate the post processor for a laser cut that generates a file with the extension .gcode?

In my V1 post processors there are processors for both .ngc and for .gcode files.

From the description above, with V2 processors I will now only have one file extension associated with both cnc and laser toolpaths. That will be .ngc. Correct?

I find that I frequently forget to add the tool name and speed to my toolpath file in Vectric so I decided to try and add that to the gcode file by editing the post processor file. I added the following statements to a copy of the post processor.

Just after the FILE_EXTENSION = “ncg” statement
POST_NAME = “OneFinity (inch_Rex)”

Just after the begin REVISION_COMMENT statement

  • Add tool name, tool notes, & router speed to header
  • By Rex Hanson 31Jan2022

“%”
“(VECTRIC POST REVISION)”
“([REVISION])”
“%”
“( Tool: [TOOLNAME])”
“(Tool Note: [TOOL_NOTES])”
“(Spindle Speed: [S])”
“%”
“%”

When I install the edited post processor file into VCarve it takes it just fine.
When I save a tool path it runs fine and creates the following statements at the top of my gcode file:

%
(VECTRIC POST REVISION)
(6BDF1E92470D996358027BC36CAD5196)
%
( Tool: Tapered Ball Nose (6.2°, Tip 1/64 - 1/4"))
(Tool Note: Amana 46280-S)
(Spindle Speed: S19000)
%
%

This all seems good, except there are two problems. The first is that when I try to load it onto my OneFinity machine I get the following error message:

Level Location Message
Error 0 Invalid character: ‘)’ At: /var/lib/bbctrl/upload/Test new PP_Inlay Plug_1-Pocket Texas Plug.ngc:5:1
  • 1 {“message”:“Unable to read file - doesn’t appear to be GCode.”,“code”:400}

The other problem is that if I examine rest of the gcode it appears that all of the moves have different values.

Anyone know what I’m doing wrong?

Thank you!

Problem Solved! At least for now.

The OneFinity controller doesn’t like the degree symbol or nested parenthesis. And since I had used them in my TOOLNAME and TOOL_NOTES I had to replace them with something else in the VCarve database.

So if you want to add those items to the top of your gcode so you will know which tool to install and what speed to set it at you can add the following lines of code just above the header section in your post processor.

“%( Tool: [TOOLNAME])”
“%(Tool Note: [TOOL_NOTES])”
“%(Spindle Speed: [S])”

The result looks something like this at the top of your gcode:
%
(VECTRIC POST REVISION)
(4AB4D9D91138E11D82267218CE3CAEF4)
%
%( Tool: Engraving - 30.0deg, Tip 0.05, 1/4")
%(Tool Note: Amana 45705 60 deg V-bit)
%(Spindle Speed: S22000)
%

3 Likes

Do you know, if by doing this, if the display on a Onefinity will display the tool identity?

If you open up the help file for the post processor editing in Vectric, you will find a list of variables. To get the tool number to display you will use [T].

I did the exact same thing and got the same error message when trying to send it. You’re correct, it doesn’t like the degree symbol. I removed it and deleted all toolpaths that caused the error but still, everytime I send a toolpath it errors the same way.
If I just keep going back in and double clicking the toolpath I want, it eventually grabs it. Sometimes it takes as many as 10 times before it works. Did you have that issue, and if so, how did you correct it or remove it?

It doesn’t like parenthesis in the tool name either.

If you look closely at the error message it tells you which line caused the error. And if I remember correctly, it also tells you which character position in the line so you can figure out which character is causing the problem.

1 Like

I need to share that in the latest Vetric upgrade to 11.5 there is no post processor specifically for the laser as .gcode. They have combined the carving and the laser as one post processor. Now it just shows .ngc and it will now raise your laser to the set start height like it does with an end mill. It will move over at that height and then drop down to your set 0 height for lasering. I like it much better that way as it prevents possible crashes.

3 Likes