Laser job preview and post processor drop down

Post Reply
jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Laser job preview and post processor drop down

Post by jamin35008 »

First, wondering about the laser module job preview. I have several laser toolpaths with different power settings but the preview shows the same darkness for every toolpath no matter what the power setting.

Second, why won't my post processor display in the select laser post processor drop down when its in the MypostP folder? Its displayed and works if its in the general post processor folder and the MypostP folder is empty.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Laser job preview and post processor drop down

Post by Adrian »

Have you got the LASER_SUPPORT = "YES" statement in your post processor?

It works ok for me in My_PostP in the dropdown within the toolpath and with the normal toolpath save.

jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Re: Laser job preview and post processor drop down

Post by jamin35008 »

Yes. I made sure I added that and restarted vcarve ans still nothing in the drop down for post processors.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Laser job preview and post processor drop down

Post by Adrian »

Does it display as the only post processor if you go to the Save Toolpaths dialog outside of the toolpath?

jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Re: Laser job preview and post processor drop down

Post by jamin35008 »

I have 7 post processors that I use on a routine basis. They are all based off of the GRBL inch post processor but each with different tape splitting gcode amounts.

The new laser post processor I'm trying to use is the openbuilds. When this post processor is in the MypostP folder alone it will display in the laser post processor drop down and the save toolpaths post processor drop down and I'm able to save the laser toolpaths from either location.

When I add the GRBL post processors back into the MypostP folder with the openbuilds post processor the openbuilds post processor will not display under the laser post processor drop down however it will display under the save toolpaths drop down with the other post processors I added to the MypostP folder. This time however if I select the openbuilds post processor and try to save the laser toolpaths I get the "error occurred, check the post processor you're using is compatible" dialog box.

gregk
Vectric Staff
Posts: 373
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: Laser job preview and post processor drop down

Post by gregk »

jamin35008 wrote:
Tue Aug 25, 2020 4:38 pm
I have 7 post processors that I use on a routine basis. They are all based off of the GRBL inch post processor but each with different tape splitting gcode amounts.

The new laser post processor I'm trying to use is the openbuilds. When this post processor is in the MypostP folder alone it will display in the laser post processor drop down and the save toolpaths post processor drop down and I'm able to save the laser toolpaths from either location.

When I add the GRBL post processors back into the MypostP folder with the openbuilds post processor the openbuilds post processor will not display under the laser post processor drop down however it will display under the save toolpaths drop down with the other post processors I added to the MypostP folder. This time however if I select the openbuilds post processor and try to save the laser toolpaths I get the "error occurred, check the post processor you're using is compatible" dialog box.
The Openbuilds post-processor that we ship inherits from Grbl_inch.pp. When you place it alone in MyPostP folder, it will look for Grbl_inch.pp in PostP folder. However once you copy your Grbl post-processors to MyPostP folder, it will take Grbl_inch.pp from MyPostP. Perhaps that other Grbl_inch.pp is different and that is causing the error? I hope this helps,

Greg K

jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Re: Laser job preview and post processor drop down

Post by jamin35008 »

Greg,
Should I try tape splitting the openbuilds post processor instead of the GRBL then? Do you think that might solve the issue?

Do you know if there is an issue with the laser preview and all power settings showing the same darkness?

gregk
Vectric Staff
Posts: 373
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: Laser job preview and post processor drop down

Post by gregk »

jamin35008 wrote:
Wed Aug 26, 2020 1:22 am
Greg,
Should I try tape splitting the openbuilds post processor instead of the GRBL then? Do you think that might solve the issue?
Do you need tape splitting when using openbuilds? If you were happy with how it worked when it was alone in MyPostP folder, then you can copy Grbl_inch.pp from PostP folder (that should be our 'stock' post) to MyPostP folder, rename it to e.g. Grbl_inch_ob.pp and then edit openbuilds postp, replacing line:

Code: Select all

POST_BASE = "Grbl_inch.pp"
with

Code: Select all

POST_BASE = "Grbl_inch_ob.pp"
This way you should end-up with OpenBuilds postp that is protected from interference of your 7 other post-processors.
jamin35008 wrote:
Wed Aug 26, 2020 1:22 am
Do you know if there is an issue with the laser preview and all power settings showing the same darkness?
There is no issue with laser preview that we are aware of. However it requires calibration. If you look at your tool definition in the tool database, there is a field called 'Maximum Burn Rate'. As described in the user manual:
This is the maximum speed at which the tool, when at 100% power, will still burn the material. This value is used for simulation purposes only. It should be calibrated to match your laser and material. A larger value will result in the simulated toolpath appearing darker.
I hope this helps,

Greg K

jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Re: Laser job preview and post processor drop down

Post by jamin35008 »

I was editing the post processor last night before reading your post this morning and was able to get things working correctly.

I kept the base openbuilds postp in the MypostP folder and then copied it 7 times and edited each post name to eg. "Openbuilds 25000 (inch) (.gcode)". 25000 represents the number of gcode per file. I kept the post base of "GRBL_inch.pp" I did this did to the other 6 also adjusting the number of lines for each one and everything seems to be working correctly.

As for the laser preview....even if it requires calibration why would a preview with two different settings come or looking the same?

Two burns, both running at 100ipm, one at 30% and one at 90% both look the same on the preview. I'm not understanding this.

gregk
Vectric Staff
Posts: 373
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: Laser job preview and post processor drop down

Post by gregk »

jamin35008 wrote:
Wed Aug 26, 2020 1:41 pm
I was editing the post processor last night before reading your post this morning and was able to get things working correctly.

I kept the base openbuilds postp in the MypostP folder and then copied it 7 times and edited each post name to eg. "Openbuilds 25000 (inch) (.gcode)". 25000 represents the number of gcode per file. I kept the post base of "GRBL_inch.pp" I did this did to the other 6 also adjusting the number of lines for each one and everything seems to be working correctly.

As for the laser preview....even if it requires calibration why would a preview with two different settings come or looking the same?

Two burns, both running at 100ipm, one at 30% and one at 90% both look the same on the preview. I'm not understanding this.
I'm glad to hear that you have it working correctly now.

I don't know what maximum burn rate is specified for your tools at the moment, but what you are seeing is possible with no/incorrect calibration.
LaserSim.png
Please take a look at attached project. This project contains 3 identical images, that are simple greyscale bars. I've used the Laser Picture toolpath, so the power changes from 0% on the left side to 100% on the right side. In each case the maximum tool power is the same, the speed is the same as well. The top one used maximum burn rate of 800, the one in the middle used 200, while the bottom one is using 350. As you can see when maximum burn rate is too high, the whole power spectrum gets squeezed in the dark region. If the value is too low, the spectrum will be squeezed in the lighter region. Something in the middle gives you power spectrum matching the colour spectrum.
If you run your laser too fast on a given material, it may not have enough power too start burning, so regardless of how much % of that power you use, the surface will remain unchanged. If you run it too slow, even with 30% of maximum power it will already burn the material very dark. Increasing power further won't make much difference to the color (but it might start a fire).
I hope that makes sense,
Greg K
Attachments
LaserMaximumBurnRateDemo.zip
(1.14 MiB) Downloaded 153 times

jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Re: Laser job preview and post processor drop down

Post by jamin35008 »

gregk wrote:
Wed Aug 26, 2020 3:29 pm
jamin35008 wrote:
Wed Aug 26, 2020 1:41 pm
I was editing the post processor last night before reading your post this morning and was able to get things working correctly.

I kept the base openbuilds postp in the MypostP folder and then copied it 7 times and edited each post name to eg. "Openbuilds 25000 (inch) (.gcode)". 25000 represents the number of gcode per file. I kept the post base of "GRBL_inch.pp" I did this did to the other 6 also adjusting the number of lines for each one and everything seems to be working correctly.

As for the laser preview....even if it requires calibration why would a preview with two different settings come or looking the same?

Two burns, both running at 100ipm, one at 30% and one at 90% both look the same on the preview. I'm not understanding this.
I'm glad to hear that you have it working correctly now.

I don't know what maximum burn rate is specified for your tools at the moment, but what you are seeing is possible with no/incorrect calibration.
LaserSim.png
Please take a look at attached project. This project contains 3 identical images, that are simple greyscale bars. I've used the Laser Picture toolpath, so the power changes from 0% on the left side to 100% on the right side. In each case the maximum tool power is the same, the speed is the same as well. The top one used maximum burn rate of 800, the one in the middle used 200, while the bottom one is using 350. As you can see when maximum burn rate is too high, the whole power spectrum gets squeezed in the dark region. If the value is too low, the spectrum will be squeezed in the lighter region. Something in the middle gives you power spectrum matching the colour spectrum.
If you run your laser too fast on a given material, it may not have enough power too start burning, so regardless of how much % of that power you use, the surface will remain unchanged. If you run it too slow, even with 30% of maximum power it will already burn the material very dark. Increasing power further won't make much difference to the color (but it may start fire).
I hope that makes sense,
Greg K
Thanks Greg! This was very helpful. I had the Max burn rate set at my spindle speed of 12000 so I adjusted that to 500 for now and I'm getting previews that now represent what my percentages are.

Another concern I have (which I replied to another post about already) is Z movement. Prior to purchasing the laser module I would use a post processor from JTech which included no Z movement. Is altering the Openbuilds inch postP possible to remove the Z movement during non 3D laser operations but not effect when using it with the router? Will selecting "Project toolpath onto 3D model" even if its not a 3D model eliminate the Z movment? The additional Z movement during laser use is adding a lot of time to each burn.

gregk
Vectric Staff
Posts: 373
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: Laser job preview and post processor drop down

Post by gregk »

jamin35008 wrote:
Thu Aug 27, 2020 4:29 pm
Thanks Greg! This was very helpful. I had the Max burn rate set at my spindle speed of 12000 so I adjusted that to 500 for now and I'm getting previews that now represent what my percentages are.

Another concern I have (which I replied to another post about already) is Z movement. Prior to purchasing the laser module I would use a post processor from JTech which included no Z movement. Is altering the Openbuilds inch postP possible to remove the Z movement during non 3D laser operations but not effect when using it with the router? Will selecting "Project toolpath onto 3D model" even if its not a 3D model eliminate the Z movment? The additional Z movement during laser use is adding a lot of time to each burn.
It is not possible to remove Z-moves in post-processor only for the laser toolpaths. "Project toolpath onto 3D model" will most likely introduce more Z-motion. I can understand that in many cases that z-movement is redundant, but the main idea with the laser module was to enable 'hybrid' 3d machining + laser. Having this z-movement allows us to stay on the 'safe side'.
I think at the moment having separate post-processors for laser with z-moves eliminated may be the way to go for 2D lasering, but care should taken. Once projection onto 3D model is involved, that approach will not work very well since it will not be possible to focus the laser on the surface of the machined model.
Perhaps in the future we will get a better solution, so the z-movement will only be used where actually necessary.
Greg K

wb9tpg
Vectric Wizard
Posts: 456
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: Laser job preview and post processor drop down

Post by wb9tpg »

Z tech heavily modified a post processor to eliminate the Z component. I did a simple change to the Post Processor to accomplish the same thing. Instead of eliminating it I reduced it to 0 by applying a scale factor.

So now I set the laser to wherever I want it above the surface and set Z=0 there. Then I run a toolpath generated with the modified post processor.

Just copy your existing post processor, rename it and change these 2 lines to:


VAR Z_POSITION = [Z|C|Z|1.3|0.00001]

VAR Z_HOME_POSITION = [ZH|A|Z|1.3|0.00001]

Easy change
Gary Mitchell
Kentucky, USA

jamin35008
Posts: 44
Joined: Thu Apr 11, 2019 3:25 pm
Model of CNC Machine: Openbuilds Lead 1010
Location: Chili, NY

Re: Laser job preview and post processor drop down

Post by jamin35008 »

I ended up taking the Jtech no Z movement postP and renaming it as:

POST_NAME = "OpenBuilds (inch) Laser (*.gcode)"

POST_BASE = "Grbl_inch.pp"

FILE_EXTENSION = "gcode"

UNITS = "INCHES"

LASER_SUPPORT = "YES"

Its now is recognized and works in the laser module as a postP and eliminated the Z movement because I kept all the parameters of the JTech postP. I will use this postP with the laser and the other postP's for the router as Gary suggested.

jjneeb
Posts: 13
Joined: Tue Aug 11, 2020 4:38 am
Model of CNC Machine: AVID CNC 4x4, Opt Lasers
Location: Gilbert, Arizona
Contact:

Re: Laser job preview and post processor drop down

Post by jjneeb »

gregk wrote:
Thu Aug 27, 2020 5:30 pm
jamin35008 wrote:
Thu Aug 27, 2020 4:29 pm
Thanks Greg! This was very helpful. I had the Max burn rate set at my spindle speed of 12000 so I adjusted that to 500 for now and I'm getting previews that now represent what my percentages are.

Another concern I have (which I replied to another post about already) is Z movement. Prior to purchasing the laser module I would use a post processor from JTech which included no Z movement. Is altering the Openbuilds inch postP possible to remove the Z movement during non 3D laser operations but not effect when using it with the router? Will selecting "Project toolpath onto 3D model" even if its not a 3D model eliminate the Z movment? The additional Z movement during laser use is adding a lot of time to each burn.
It is not possible to remove Z-moves in post-processor only for the laser toolpaths. "Project toolpath onto 3D model" will most likely introduce more Z-motion. I can understand that in many cases that z-movement is redundant, but the main idea with the laser module was to enable 'hybrid' 3d machining + laser. Having this z-movement allows us to stay on the 'safe side'.
I think at the moment having separate post-processors for laser with z-moves eliminated may be the way to go for 2D lasering, but care should taken. Once projection onto 3D model is involved, that approach will not work very well since it will not be possible to focus the laser on the surface of the machined model.
Perhaps in the future we will get a better solution, so the z-movement will only be used where actually necessary.
Greg K

I have had to make a laser only post processor as well to remove all the Z moves that i don't want while lasering. I don't know why the toolpath itself can't have a control in it so the user can simply tell it to disable Z moves when it builds the toolpath. then we could use the same post processor for both laser and spindle.

Post Reply