Shapeoko with OPT Laser

Post Reply
GlitchDesign
Posts: 6
Joined: Sat Nov 11, 2017 6:25 pm
Model of CNC Machine: Denford 6600

Shapeoko with OPT Laser

Post by GlitchDesign »

Hi,

Just wondering if there is anyone out there having success with a (Carbide 3d) Shapeoko and an OPT laser?

After a somewhat disappointing experience with the trial software ('feedrate is undefined' etc.), i eventually got a reasonable result with the .506 version (not perfect, but i would have been prepared to live with it's shortcomings).
Upon purchasing the module, since the .507 update everything has stopped working with my set up.

From looking at the code the change seems to be that an extra s0 spindle speed has been introduced, with the actual speed bumped onto the following line, so, for example:

G1Z0.000F1500.0
M4S1000
G1Y195.496

has become:

G1Z0.000F1500.0
M4S0
S1000
G1Y195.496

The result, for me at least, has been that the laser comes on when it is supposed to be off, and turns off when it is supposed to be on - popping up endless spindle dialogues in the process. Not a great (or safe) outcome.

Is anyone able to advise me on how i could remedy this? Is it something i can address by modifying the pp myself?

One other seemingly gaping omission which i found after buying the laser module was the lack of anywhere (obvious) to input the offset between the laser head and the router head. I had assumed that there would be a section in the laser tool database where i could pop in these distances and the not have to worry about it from there. I'm hoping that this functionality is there, but i just haven't managed to locate it yet Can anyone enlighten me on this?

Thanks

User avatar
Adrian
Vectric Archimage
Posts: 14504
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Shapeoko with OPT Laser

Post by Adrian »

The offset between the head and laser should be setup in your control software I would have thought. That's how it works on my machine. The Vectric software knows nothing about it other than any code in the post processor.

Does it really matter though? You zero for the laser toolpath and then zero for the toolpath with the bit so as far as code is concerned they are both in the same position when run.

GlitchDesign
Posts: 6
Joined: Sat Nov 11, 2017 6:25 pm
Model of CNC Machine: Denford 6600

Re: Shapeoko with OPT Laser

Post by GlitchDesign »

Adrian wrote:
Sat Sep 19, 2020 12:55 pm
You zero for the laser toolpath and then zero for the toolpath with the bit so as far as code is concerned they are both in the same position when run.
I guess it's a matter of semantics, but to me having to fiddle with the zero positions between ops does not really conform to Vectric's promise of 'hybrid CNC & laser machining' with the module...

GlitchDesign
Posts: 6
Joined: Sat Nov 11, 2017 6:25 pm
Model of CNC Machine: Denford 6600

Re: Shapeoko with OPT Laser

Post by GlitchDesign »

Adrian wrote:
Sat Sep 19, 2020 12:55 pm
The Vectric software knows nothing about it other than any code in the post processor.
Do you think that a laser specific post processor would be the most appropriate place to implement this offset?
I don't have a good handle on either modifying post processors at the moment, but i'm definitely interested in learning.
Adrian wrote:
Sat Sep 19, 2020 12:55 pm
The offset between the head and laser should be setup in your control software
This is the other option i have been considering. At the moment i'm using the stock Carbide motion control sotware, which is simple to use, but doesn't allow for any customization.
I've been thinking about moving over to CNC.js. If i did this, presumably i could just set up a macro that runs some gcode commands to add the offset. To me this would seem like an easier option. What are your thoughts?

User avatar
Adrian
Vectric Archimage
Posts: 14504
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Shapeoko with OPT Laser

Post by Adrian »

I don't know what your control language and software can do unfortunately. With my setup (ShopBot) I can put all sorts of direct programming commands and variables into the post processor which makes offsets etc very easy.

From what I've read on the forum about the Shapeoko type machines they are much more limited but hopefully someone who has one will chime in with some ideas.

wb9tpg
Vectric Wizard
Posts: 453
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: Shapeoko with OPT Laser

Post by wb9tpg »

GlitchDesign wrote:
Sat Sep 19, 2020 1:39 pm
Do you think that a laser specific post processor would be the most appropriate place to implement this offset?
I have implemented the offset for my laser in a customized post processor. I use a spindle mounted laser with only 0.5mm offset in X and Y but the principle is the same. I used G92 commands to do it.

In the header section of my laser post processor I added these lines
"G0[XH][YH]"
+ Now apply a temporaty 0.5mm offset for my laser alignment issue
"G92 X-0.5Y0.5"

In the footer section add this
"G0[XH][YH]"
+ Cancel the offset
"G92.1"
It'd be a good idea to add the G92.1 command to the header sections of your normal post processors to cancel any offset in case the laser toolpath didn't complete for any reason.

Just customize the offset to amount to what you need for your setup
Gary Mitchell
Kentucky, USA

ElevationCreations
Vectric Craftsman
Posts: 180
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Shapeoko with OPT Laser

Post by ElevationCreations »

Why not use a different WCS for the spindle and one for the laser?

If you know the offset of the laser from the spindle, this should be relatively easy to adjust with the homing sequence. If you home the machine and have fences to orient your work, you could effectively use G55 for your spindle TP and set G56 or any other to G59 for your laser offset TP. If you are using G54 (default) just move your X-Y by the offset and zero X-Y, and Z if you need to for the laser.

Depending on your work flow you could edit your PP to call out the G56 for the laser WCS Starting position or just have a separate g-code file for the laser TP, change from G55 to G56, then run the laser file.

Depending upon which G-Code Sender you are using, there are many different ways to achieve this. We use Intelli-G-Code which is a very adaptable sender, has large easy to read screen, and is easy to understand and set up. b-CNC is very capable and customizable. Chilipepr is a web based sender, easy to configure, but only allows for 5MB files as I recall last time we used it a few years ago, however this may have changed with updates since then.

GlitchDesign
Posts: 6
Joined: Sat Nov 11, 2017 6:25 pm
Model of CNC Machine: Denford 6600

Re: Shapeoko with OPT Laser

Post by GlitchDesign »

wb9tpg wrote:
Sat Sep 19, 2020 3:34 pm
I have implemented the offset for my laser in a customized post processor. I use a spindle mounted laser with only 0.5mm offset in X and Y but the principle is the same. I used G92 commands to do it.
This sounds very do - able.
Thanks. I'll look into it...

GlitchDesign
Posts: 6
Joined: Sat Nov 11, 2017 6:25 pm
Model of CNC Machine: Denford 6600

Re: Shapeoko with OPT Laser

Post by GlitchDesign »

ElevationCreations wrote:
Sat Sep 19, 2020 4:53 pm
just have a separate g-code file for the laser TP, change from G55 to G56, then run the laser file.
If I do go down the road of using a different sender (which i will inevitably do sooner or later), i'll definitely look into this. So the different work co-ordinate systems are stored in the software, and i can switch between them using MDI or macros?
Thanks for the tip. Sounds sensible...

ElevationCreations
Vectric Craftsman
Posts: 180
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Shapeoko with OPT Laser

Post by ElevationCreations »

GlitchDesign wrote:
Sat Sep 19, 2020 5:45 pm
So the different work co-ordinate systems are stored in the software, and i can switch between them using MDI or macros?
Thanks for the tip. Sounds sensible...
It uses two different coordinate systems, machine coordinates ( in reference to machine home ) and work offset coordinates - stored in the controller. If you look at the gnea/grbl on Git Hub Wiki for GRBL v1.1 commands, it explains it in a high level overview. The sender just references what is stored in the controller.

When going between setups on our machines we just select the WCS from a drop down menu in the sender before running the TP. How you achieve it will be dependent on what type of workflow you desire. We try to stick to the KISS method.

Post Reply