Laser Module with Shapeoko

[DanSexton]

Just installed and tested the new Laser Module and have a couple questions / issues, I have a Shapeoko XXL with a JTech 7W laser. I am using the Shapeoko (mm) post processor.

My tool settings are Power: 7 Watts, Kerf: 0.0075 inches and Power:100%, Number of passes:1, Move speed: 80

I am using the Cut and Fill with "Cut On" selected.

The issues I have are:

1. My gcode loader (CNCjs) gives me a warning about not having a default feed rate. It continues on anyway.

2. My Image is a single line with a few angle changes but in the 3D preview it shows it as a very, very thick line.

3. Instead of starting at the beginning of the single line and burning to the end of the line it does a z hop at each intersection, moves to a new spot and moves back to the z0 and makes another cut and repeats until complete. The result is that the line does get burnt correctly but at each stop and start point it leaves an oversized burnt dot thus ruining the image.

4. I tried a small image with Hatch fill but instead of filling it just drew lines about 2.5mm apart. The preview shows a completely filled image.

It seems to think my laser is really wide in the previews and cutting.

I would provide some pictures but not sure how to do so on this site since I don't have any public storage.

As an aside I have used the etching tool using the driver and settings provided by JTech and it works just great. It won't let me use the driver for the new laser tools however.

Any suggestions on what I can try next or am I using the wrong processor? When I downloaded it I did select Shapeoko and Jtech.

Thanks.

[Guest]

Edit to my post. The thick line was due to my stepover being 0.075 instead of 0.0075. The issue of the hopping and burnt lines persists.

[Adrian]

You don't need public storage to add pictures. When you type a reply/post you can drag and drop a picture into the message or use the Attachments tab underneath the "Save draft", "Preview", "Submit" buttons to manually upload a picture.

[EdwardP]

Hi Dan,

Can you drop an email to support@vectric.com and we can take a closer look at the issues you are seeing? The Shapoko machine with up-to-date grbl (1.1 or later) and a j-tech laser should work fine and the support team will hopefully get you up and running. When you drop us an email can you also ensure that you have enabled the grbl controller's laser mode ($32=1) before create images of your output as this will produce the most consistent results but must be set manually (please see https://github.com/gnea/grbl/wiki/Grbl-v1.1-Laser-Mode for more details on this).

For others reading this post, please don't forget that our free trial editions (e.g. https://www.vectric.com/free-trial/vcarve-pro) include a test mode and sample files for the laser module so you can test your CNC setup for any problems before you purchase.

Thanks,

E

[shaunlb]

edwardp

With the Shapeoko do we have to use the standard .grbl post processor? When i try to use any other Shapeoko post processor i get a notification that tells me

"an error occurred while outputting toolpath... Check the post-processor you're using is compatible with the toolpath you're trying to output. "

[EdwardP]

Hi Shaun,

Thanks for highlighting this one. That message usually indicates that the post processor you are using doesn't have the correct structure to support the new laser toolpath types. The most common reason for this with a supported machine type (like the shapoko) is that the post is from an older version (V10 or earlier) - perhaps sneaking in via your My_PostP folder?

In the general toolpath saving list on the toolpath tab we show all available posts - laser and non-laser enabled - because we cannot know in advance what type of toolpath you are planning to save. But if you use the drop down list of post-processors on the Laser Cut & Fill toolpath form specifically, that will show you *only* those posts that explicitly support the laser toolpath types. To be clear, these the *same* posts - they have just been singled-out of the main list as being laser capable.

One other important note is that I *think* we may have inadvertently missed the imperial (inches) version of the Shapoko post from the laser set in the very first release. Please ensure that you update to the latest version of V10 (V10.503 or later) and you should see this includes laser enabled Shapoko specific posts (inch or mm depending on your preference) - you should now be able to use the same post for routing and lasering.

I hope this helps clarify a few things for others too.

E

[shaunlb]

Alright, i just went ahead and removed all vectric products and reinstalled so that I would have the current provided PP from Vectric. I make sure that I have set the .grbl settings to laser mode ($32=1). Now the Post can be saved in Vcarve as a post but when I go to run the code it states a warning about not having a default feed rate and the program does not continue on. No movement from machine and the program does not continue running. I am using Carbide Motion (Shapeoko Default Motion Control Software). I also found that you have to create the laser tool initially (tried using what it came up with by default and that definitely did not work) but some of the default characteristics do not make sense to me. I apologize for being a pain, but this tool, when working properly, can really streamline my workflow.

[EdwardP]

Hi Shaun,

Thanks for the additional feedback. The missing feedrate is a mistake in the imperial units (inches) version of the grbl post from which the shapoko one derives. Sorry about that, we have fixed this for the next patch (due later today). In the meantime, I think you should be able to correct it yourself if you cannot afford to wait for the patch.

In Grbl_inch.pp file within your Postp directory:

Code: Select all

begin PLUNGE_MOVE

"G1[Z]"

should read:

Code: Select all

begin PLUNGE_MOVE

"G1[Z][F]"

You can find the location of your PostP folder by selecting File->Open Application Data Folder command from the main menu. It is typically: C:\ProgramData\Vectric\VCarve Pro\V10.5\ for a default installation of VCarve Pro 10.5, for example.

While you are in that location, the lack of default lasers can also be worked around by importing the example set into your tool database - these are ones we have created using 3.8w and 6w diodes we have on our test machines here. In the tool database window please click the 'import a tool database' button, it has the folder icon. You should find a 'laser_tools.vtdb' file in the ToolDatabase folder in that same application data location. Please do treat these tool settings as examples only and note they may need to modified for your machine configuration and materials.

I do hope that this helps,

E

[DanSexton]

Still having an issue with the missing feed rate.

From what I see both Shapeoko_mm and Shapeoko_inch derive from GRBL_mm with the inch file merging additional header lines. I have created the gcode from both the mm and inch processors and I still get the missing feed rate reported on the G1Z0.000 line in each file.

Not sure if it is my CNCjs that is causing the issue or something else. The behavior I get is:

- Zero machine and load the gcode
- Run
- Laser moves to first cut point and raises the Z +5. Pauses with the error of the missing feed rate.
- Press continue
- First cut continues but at the wrong Z+5 height.
- Continues to subsequent cuts and they are all at the correct Z height
- After completing the cuts I run it again and it works fine without the warning or the bad first cut.

Any suggestions on what I should try next? I am running 10.505

[wb9tpg]

I'll attach my modified Grbl PP file that works. Neil Frerari did a lot of work on the PP on the Carbide3D site and found the precision is not high enough on the standard PP with arcs enabled on GRBL. Put it in your My_PostP folder to try it

[cwjohn67]

I purchased / installed the laser module on 7/18 for use with Pro 10.5 build 504. I have a Shapeoko XL and J Tech 4.2W laser that I have been running with the J Tech PP in vCarve and USGS as the sender. For Comparison I ran a project with both post processors. the vCarve / J Tech / USGS combination completed the project in 7 min 5 seconds. the vCarve / laser module / Shapeolo in PP/ Carbide motion sender combination completed the project in about 40 minutes the time sheet said it should complete in 14 min 9 seconds.

I did have to add the F feedrate in the gcode. I also compared it to the gcode from the J Tech PP - J Tech uses a M4S0 / M4S*** (appropriate speed / power) combination for the laser and Vectric uses M4 / M5. There is a lot of delay between moves, possibly because it takes longer to shut off than spin down? I edited the laser module gcode to use the M4S0 / M4S*** and it trimmed the run time to about 30 minutes. I took some video of how the laser was moving but didn't want to drop that here if there is something obvious I'm doing wrong.

Any thoughts why the timing is so far off or how I can tune my workflow to get it in line with the time sheet estimate?

Thanks
Clint

[DanSexton]

I'll attach my modified Grbl PP file that works. Neil Frerari did a lot of work on the PP on the Carbide3D site and found the precision is not high enough on the standard PP with arcs enabled on GRBL. Put it in your My_PostP folder to try it

That processor has laser support = "no", so until he posts another with laser support it won't help in this circumstance

[wb9tpg]

I'll attach my modified Grbl PP file that works. Neil Frerari did a lot of work on the PP on the Carbide3D site and found the precision is not high enough on the standard PP with arcs enabled on GRBL. Put it in your My_PostP folder to try it

That processor has laser support = "no", so until he posts another with laser support it won't help in this circumstance

oops - my apologies. There is one included that reduces Z motion to 0. I use it most of the time. I'd customized for CNCjs with $32=1 (laser mode on) and with the %wait directive

[DanSexton]

Thanks Bill, the No Z seems to be ignoring whatever I set for a speed setting on the laser tool.

The whole idea is that you don't have to keep switching between processors for different tools, or at least that was the appeal to me.

My previous post about it getting hung up on the feed rate is the biggest problem. I fixed a lot of the quality issues by adjusting my speeds but the initial cut still gets messed up by the feed rate error.

I use a lot of Neil Frerari's macros and do remember using his post processor before. I do wonder if it is such an obvious issue why doesn't Vectric fix their processor?

I have a support ticket submitted and I requested a follow up a couple days ago but have not heard anything back. I know the covid thing is slowing things down for them but I hope they get this resolved.

[DanSexton]

I purchased / installed the laser module on 7/18 for use with Pro 10.5 build 504. I have a Shapeoko XL and J Tech 4.2W laser that I have been running with the J Tech PP in vCarve and USGS as the sender. For Comparison I ran a project with both post processors. the vCarve / J Tech / USGS combination completed the project in 7 min 5 seconds. the vCarve / laser module / Shapeolo in PP/ Carbide motion sender combination completed the project in about 40 minutes the time sheet said it should complete in 14 min 9 seconds.

I did have to add the F feedrate in the gcode. I also compared it to the gcode from the J Tech PP - J Tech uses a M4S0 / M4S*** (appropriate speed / power) combination for the laser and Vectric uses M4 / M5. There is a lot of delay between moves, possibly because it takes longer to shut off than spin down? I edited the laser module gcode to use the M4S0 / M4S*** and it trimmed the run time to about 30 minutes. I took some video of how the laser was moving but didn't want to drop that here if there is something obvious I'm doing wrong.

Any thoughts why the timing is so far off or how I can tune my workflow to get it in line with the time sheet estimate?

Thanks
Clint

Did you make any progress on this Clint?

I think there is an issue of generating the gcode when it is using the Laser tool. Using Shapeoko_mm processor is simply using the grbl_mm processor since it is a just a merge from it,

If I create a profile cut with an end mill the processor creates the first G1 line as "G1Z-3.175F762.0" which includes the feed rate.

However if you use the same processor on a laser tool path it generates "G1Z0.0000" for the first G1 line, this seems like a canned line that is inserted in every laser tool path.. This does not have a feed rate so it generates an error that you can skip over. Problem is that since it errored it did not set the Z to 0.00 and since a previous line had set Z to 5.00 the first cut is too high.

This is an example:

G0X0.000Y0.000 - MOVE 0,0
G0X87.231Y119.766Z5.080 - MOVE to first X and Y coordinates and set Z to 5.080 To clear material
G1Z0.000 - TRY TO SET Z to 0.00 BUT GENERATES AN ERROR SINCE NO FEEDRATE IS INCLUDED
M4S1000
G1X88.220F20320.0 - STARTS FIRST CUT AND SETS THE FEED RATE BUT Z AT WRONG HEIGHT
G1X88.273Y119.784
G1X88.477Y119.879
G1X88.602Y119.957
...
...
...
M5 - TURN OFF LASER
G0Z5.080 - SET Z TO CLEAR BUT IT IS ALREADY HERE
G0X87.862Y120.338 - MOVE TO NEW POSITION
G1Z0.000 - THIS NOW WORKS SINCE A FEED RATE (F) WAS ENTERED EARLIER
M4
G1X86.421F20320.0
...
... SUBSEQUENT CUTS ARE NOW AT THE RIGHT Z HEIGHT

So what I have to do is manually move the Feed rate to the correct line.

Hope this helps anyone else having the issue and please let me know if I have something wrong or if I am doing something incorrectly.