Information on our Vectric Laser Post Processor
We have been asked by a lot of people to make a post processor to the Vectric Software so it can be used with the laser. You ask and you shall receive! We started one for the X Carve, but it should not really have anything that specific in it to make it unusable for other machines as well. If you would like to modify it the source file can be edited with a standard text editor pretty easily. We have made now specific versions for different machine controllers. If you have a new post processor for another controller that you would like to share, just let us know!
This post processor will work with all of the Vectric Products including Cut2D, V Carve, and Aspire. It works with the desktop and the Pro versions.
The basic concept is that you set up a tool in V Carve Pro (or other Vectric software) that has the laser parameters to it (the spot size is the drill bit width). Then, you draw in V Carve Pro (or other vectric software) to get the file that you want. When you make your G Code, the post processor will change all of the “retract” portions in the file where the spindle moves up to a laser OFF command. Viola!
We have a couple of versions depending on the controller you use. Here are the download links:
*Right click “save link as” versus clicking the link *
GRBL 1.1 – Dynamic Laser Mode M4 & No Z (X Carve, Shapeoko 3, etc.)
GRBL 0.9- With Z Older Machines (X Carve, Shapeoko 3, etc.)
GRBL 0.9- Older Machines No Z Version (X Carve, Shapeoko 3, etc.)
MACH 3 – M11p1/M10p1 option
MACH 4 – Vector Laser Mode – No Z
STEPCRAFT (UCCNC) Relay Option
UCCNC (Stepcraft) PWM Option
UCCNC CNC4 Newbies PWM Option
3D Printer (Using Fan Control M106/M107)
3D Printer (Using Fan Control M106/M107) with ARCS
ShopBot (Using OP5 Connection)
Axiom Precision Pro/Basic
Axiom Elite Machines
Probotix (with M68 power control command)
*Note: These post processors will probably work for a lot of different machine controllers. If you are having problems, then let us know and we can help modify it for your machine.
Now we will cover how to set it up.
1. Set up the Post Processor
Put the post processor file in the directory: C:\ProgramData\Vectric\VCarve Pro\V8.0\PostP
You need to click on your c:\ drive and on the “view” tab you need to click on “hidden items” to view the program data folder. Then click on Vectric and your product folder to browse down to the PostP folder.
If you have the newer versions of Vectric, then you can install the post processor from inside the tool itself.
2. Set up Your Tool
First you need to have a tool for your laser with the correct parameters. In the “Tool List”, make a new tool for the laser. For the “Diameter” put the spot size for the laser. For the different lasers you will have different spot sizes and it depends on your ability to focus as well. Here are some values you can try. If you notice on the fill engrave that there are a lot of space between the lines, then make the numbers smaller until you don’t have spaces anymore.
Standard High Efficiency Lens:
- 1W laser: 0.004″ (0.1mm)
- 2W laser: 0.006″ (0.15mm)
- 2.8W laser: 0.007″ (0.18mm)
- 3.8W laser: 0.011″ (0.28mm)
- 4.2W laser: 0.011″ (0.28mm)
- 7W laser: 0.011″ (0.28mm)
High Resolution Lens Option:
- 1W laser: 0.004″ (0.1mm)
- 2W laser: 0.0055″ (0.14mm)
- 2.8W laser: 0.006″ (0.19mm)
- 3.8W laser: 0.006″ (0.19mm)
- 4.2W laser: 0.006″ (0.19mm)
- 7W laser: 0.006″ (0.19mm)
- 14W laser: 0.006″ (0.19mm)
- 24W laser: 0.006″ (0.19mm)
You can then set the feedrate here for the tool. You can make different tools for different feedrates, or you can modify the tool whenever you want to change the feed speed. Here are some parameters we have:
3. Make Your Project
Do what you normally do in your Vectric Software to design. Use your tool from the previous setup in your drawing. Here is an example we have:
3. Set Up your Toolpath
Change your Z settings to reduce the Z movement of the machine. The laser will be on during the “plung” and the safe Z moves. You need to eliminate these or the laser will leave a “dot” where it stops to move Z because it will burn.
Set your toolpath settings for your project and then select the post processor from the drop down box. It will be named based on which post processor you downloaded.
4. Save G Code and RUN on your machine!
It is pretty easy. Here is the result from this project:
There are a lot of cool features in the Vectric Software to try out. Here is a filled engrave example:
So there it is. If you have questions, then let us know and we can help to get your vectric software working.
Can the spindle speed be used to control the power of the laser in this post processor?
Yes, the spindle speed is the laser power when you have PWM on your machine. The spindle RPM will be placed into the code line as a “S” parameter which will set the PWM output for the laser power.
Do you have a metric version? MM instead of Inches?
Yes. Added it to the drop down list in the download section of the page.
You are in Germany- I´m in Germany and I think I have some questions later to CNC and laser-
Hi, I am using this post processor to generate gcode for a plasma cutter, everything is working fine except i need some dwell times for torch on and torch off, in the gcode. Right now i am generating gcode and than editing the gcode manually. Can i edit the post processor to get it to create dwell or do i have to use mach3 to create dwell time. I am using spindle output 1 pin 17 with a relay to turn the torch on and off. I don’t have a z axis, the torch is at a fixed height.
Hi Leroy- You can put in a G4 P# command (where # is the time in seconds you want to dwell). Just edit the post processor in a text editor. When there is a M3 command, then put a G4 P# command on the next line. Also, put a G4 P# in the “retract” section after the M05 command. This will generate the g code file you are looking for.
Great idea, thanks !
So If I understand correctly, I plug the laser in the same socket as I usually plug my spindle, and it will switch power off where the spindle usually goes up ?
Yes. It will turn on the laser when the spindle normally does the “plunge” and then turn it off when it does the “retract”. Works pretty good!
Thanks a lot, works fine. very Helpful. JUST PERFECT
I must be missing something… I click on the link for the HD Shark download and I simply get a new page – no download of a file to save to the PostP folder….
Hi Tony- You need to right click on it and press “save link as” to download it.
Thank you ???
I have followed all of the instructions and cannot get this work.
Any idea if this works for Trotec or ULS lasers?
Doubt it. The Trotec and ULS have their own software for running the laser.
Do any of these work with a Jtech laser with a DAC board set up on the A axis work?
If you are using mach3 and your have your output for M03 set to an output pin to turn on and off the DAC, then yes it will work. Just set your laser power by jogging your DAC to your desired level, and then run the program generated by the post processor that will turn the DAC on and off for the engraving.
what is the difference in these?
A) GRBL – (X Carve, Shapeoko 3, etc.)
B) GRBL – No Z Version (X Carve, Shapeoko 3, etc.)
C) GRBL – Dynamic Laser Mode M4 & No Z (X Carve, Shapeoko 3, etc.)
A) For older versions of Firmware (<1.1f) and includes a Z component (allows for Z path following)
B) For older versions of Firmware (<1.1F) and does not include Z component.
C) For GRBL 1.1F and newer Firmware that has Laser Mode ($32=1).
If you have a new machine with GRBL 1.1F, use the GRBL - Dynamic Laser Mode and make sure you have your firmware setting $32=1.
I have downloaded the Mach3 version for my Blacktooth Laser.
All my tool paths seems to be correct but the laser itself does not switch on. My laser is wired to the Z up/down movement (Pin 16 through the relay) instead of the spindle.
Will it be easier to change the pp instead of rewiring the whole machine.
I’m using V-Carve Pro 9.5 with Mach 3.
You can download and edit the post processor. In the “retract” section, put your Zup movement and in the “plunge” put your Z down movement. Just download it and edit in a text editor to make changes.
Do I understand right? The Vectric Laser Post Processor does not work with VcarveDesktop? I must be misunderstanding. Thanks
It will work on all vectric products. We just happen to have V Carve Pro, so we mentioned it. It will work on both pro and desktop for Cut2D, V Carve, and Aspire.
awesome stuff i was able to sync it up with my aspire and shapeoko 3xxl. Love it.
please help me. i’m new and i don’t know what post processor is CNC 3018 woodpecker 3.2, brgl 1.1f
thank in advance
Use this one: “GRBL – Dynamic Laser Mode M4 & No Z”
Getting ready to try my first test…. Do i need to turn the laser on before I send the code with picsender or will it turn on automatically?
Have the power to the laser turned on with both fans running. Keep it in “input control mode” with the small switch in the front to the right labeled “TTL”. The program will turn on and off the laser when needed.
If I use this with V-Carve pro, do I need Lightburn as well?
No, you do not need lightburn if you just want to do vector engravings. However, lightburn will be able to do pictures as well. Both are very good programs.
can you say me how you do this filled engrave with vectric?
In the quick engrave toolpath you have the option to choose “fill”. Select this and then define your stepover and your angle of the fill. You can do an offset or a hatch. Directions are on the top of this page where it shows how.
Was having a weird problem with loaded gcode, usually it would just map out a graph type line in toolpath visualisation that exceeded bed limits, other times it would load and the toolpath visualisation was correct.
Having looked at the generated code I found there is no explicit setting for G91 or G90. Have added a G90 to the header section and now it always loads properly.
I started to follow the instructions for making a tool, but in the Tool Type dropdown list there is a Laser Cutter type. I assume this showed up after the example above was given. Have you given instructions on using it, maybe on another page, or is this the latest?
We are going to test the “laser tool” function to make sure it works with all of our post processors. Right now, we suggest using an end mill where the RPM value is the laser power. We will update these instructions later for using the laser tool.
Hi, I have problems with this Vectric ASPIRE Laser Post Processor.
the problem is that it shoots the laser a few milliseconds before the movement of the axes begins
.and burning a point for the rest works perfect, you could regulate the delay the shot.
If you are using mach3, make sure your spindle delay is set to zero. Check this on any controller you may be using. If this is still an issue and you are using Mach3, then try to use the M11P#/M10P# direct outputs to control the laser. You can see the details on setting this up here: https://jtechphotonics.com/?page_id=1436
I purchased the Jtech 2.8 Watt laser and have it all hooked up. I downloaded the Postprocessor for Vectric and have Mach3 turning laser on and off, everything is working great. However,…..I want to move to the next step of controlling the laser power. Right now my Laser is either ON or Off.
My HobbyCNC Pro board does not have PWM output capability.
Is the DAC-PWM board my next option? Mach 3 cannot control laser power by itself, is that correct?
I just want to make sure I’m on the right path.
You can use mach3 to control laser power by setting up the PWM output. You can see the details in this post here: https://jtechphotonics.com/?page_id=1436
Try messing around with it to see if you can get it to work with your machine. The DAC-PWM board is a much harder way to go versus just getting PWM to work with mach3 outputs.
V-Carve has a laser cutter in the drop down box. Still set it up as an endmill?
We are working on getting the “laser cutter” tools to work soon. I’ll update the instructions when we have all of the post processors verified that they work with the new laser tool dropdown. As for now, we know they work using the “endmill” option.