I’m using a Genmitsu 4030 (GRBL 1.1).
Whatever I do, the (Get Position) origin is set at -343,-281 (relative to home, I assume).
I don’t know where this setting came from. If I set the machine origin manually to something else (with Candle) it makes no difference.
Set Origin, Clear Origin have no effect.
Why do I care ? I want to use the same machine for CNC routing and for lasering, and there needs to be a 12.5mm offset between the origins (due to laser/router size), so I want to be able to set the physical origins manually.
The documentation for origin setting and modes is somewhat confusing, but I don’t think that this is the problem.
Take a look at this documentation for common GRBL configurations, specifically about negative workspace systems:
Common GRBL/GCode Setups - LightBurn Software Documentation
I read through that before. Did not help.
The problem is that LB has found some specific origin value, and will not let it go.
What I need to know is how to change this value.
Don’t see how negative workspace issues are the problem - it seems to use this origin value just fine, but will not allow it to be changed.
Can you document what you actually tried thus far? It’s odd that it wouldn’t do anything at all.
I’ve tried everything I can think of. The problem is that I can see no way to define the physical origin.
I would expect one corner of the workspace to be at HOME (0.0) and the other one to be either user-definable (yes please) or at least fixed at the opposite corner of the physical work space.
But, the second point seems to be a semi-arbitrary value. Although, interestingly, quite close to a value I’ve used with other software. Could it be stored in the interface after powerdown ? If so, when and how would LB read it ? It does not change (-343,-281).
Essentially, my question reduces to: how do I define/change the physical origin starting position ?
I’m confused. The linked article expressly covers that process but you’re saying it’s not doing what you expect.
What specific changes have you tried and what were the results? You’ll need to be specific or else it’ll be impossible to arrive at the core problem.
If you’re not certain what to do then just state so and we can start from ground zero.
I’m also confused but since I am new to this I will do it your way.
SInce my machine is not among your specified units, I will follow Other machines
Pressing the Home button - moves to top right (0,0)
G0 X0 Y0 - moves to current physical origin ( -343,-281)
G0 X10 Y10 - moves to -333,-271 so we have positive coords
So it says " You simply set the origin in LightBurn to match the machine origin discovered above". Not clear how I do this. I tried Move/SetOrigin - nothing happens. Also, since I want to change the origin, not sure why I would do this.
Alas - my original question was how to CHANGE the physical origin. Why do I want to do this ? If I don’t, the unit will hit the limit switches before it reaches the limits of the workspace, because the stated physical origin is inside the physical workspace. (343,281) is inside (0,0,400,300).
.
So to confirm, your machine has homing switches and is self homing to top-right?
Please provide the following:
- After homing, run this in Console. What is the output?
?
- Use the jogging controls to move the laser to the opposite corner. Repeat command from above. What is output?
- Screenshot of Edit->Device Settings
- Run these commands in Console and return output:
$I
$$
$#
1 Like
So to confirm, your machine has homing switches and is self homing to top-right?
Correct.
Please provide the following:
- After homing, run this in Console. What is the output?
?
<Idle|MPos:-3.000,-3.000,-3.000|Bf:15,127|FS:0,0|
WCO:-343.000,-281.000,0.000>
- Use the jogging controls to move the laser to the opposite corner. Repeat command from above. What is output?
By opposite, I assume you mean bottom left. Not sure if you want me to hit the limit switches, but I assume you do (otherwise unclear where I should stop).
<Idle|MPos:-431.856,-301.744,0.056|Bf:15,127|FS:0,0|Pn:XYZ|
WCO:-343.000,-281.000,0.000>
-
Screenshot of Edit->Device Settings
-
Run these commands in Console and return output:
$l
$l
error:2
Numeric value format is not valid or missing an expected value.
$
$
[HLP:$$ $# $G $I $N $x=val $Nx=line $J=line $SLP $C $X $H ~ ! ? ctrl-x]
ok
$#
$#
[G54:-343.000,-281.000,0.000]
[G55:0.000,0.000,0.000]
[G56:0.000,0.000,0.000]
[G57:0.000,0.000,0.000]
[G58:0.000,0.000,0.000]
[G59:0.000,0.000,0.000]
[G28:0.000,0.000,0.000]
[G30:0.000,0.000,0.000]
[G92:0.000,0.000,0.000]
[TLO:0.000]
[PRB:0.000,0.000,0.000:0]
I think you botched one of the commands. Can you rerun this one?
$$
You have an offset configured but not sure why these values. I’m going to assume your 400x300 work area is correct. This may require a tweak after you provide the $$ values but let’s try this.
Run in Console:
G10 L2 P1 X-400Y-300
$10=0
$H
?
The $H should make it home so watch out for that. Please return results.
Home position should report as somewhere around 400,300 if things are good. Jogging to bottom-left should report 0,0.
from HOME
$$
$0=10
$1=255
$2=0
$3=0
$4=0
$5=0
$6=0
$10=3
$11=0.010
$12=0.002
$13=0
$20=0
$21=1
$22=1
$23=0
$24=25.000
$25=500.000
$26=250
$27=3.000
$30=255
$31=0
$32=1
$100=160.000
$101=160.000
$102=160.000
$110=2000.000
$111=2000.000
$112=2000.000
$120=300.000
$121=300.000
$122=300.000
$130=420.000
$131=310.000
$132=110.000
ok
G10 L2 P1 X-400Y-300
G10 L2 P1 X-400Y-300
ok
$10=0
$10=0
ok
$H
$H
ok
?
?
<Idle|WPos:397.000,297.000,-3.000|FS:0,0|WCO:-400.000,-300.000,0.000>
ok
Actually that looks promising - if I do a GoToOrigin, it looks good.
?
?
<Idle|WPos:0.000,0.000,-3.000|FS:0,0|Ov:100,100,100>
ok
But - you will know what it means - can you give me a clue ?
Can you confirm that bottom-left is now 0,0 and that 400,300 is top-right? You may hit the limit switches if you go all the way.
I’m curious about this, though. This seems to indicate that your laser expects the work area to be 420x310. If so, I suspect 0,0 is not going all the way to the bottom-left corner.
In any case, test the various functions of the laser:
- Make sure jogging controls are working correctly
- Try framing a job
- Run a test burn
Do things work properly?
Hi - we’re kinda getting to the edge of my knowledge here (early days).
I don’t really know how you define bottom left and top right except as home and origin.
The home position is now 397,297. This sounds right, as there is a 3mm backset following the limit switch detection.
The origin position is of course 0,0. There are a few mm to go in Y and about 22mm in X before it hits the limit switches. This is consistent with your 420 value but not the 310. But, it’s enough for me.
- Jogging seems OK.
- Don’t know what “framing a job” means. (Sorry).
- I’ll try some tests and report back, but I’m hopeful.
What tests would be good ? I’ll try and burn a 10,10,390,290 square.
Hi - my 10,10,390,290 square did what I would expect it to, so I assume we are good.
One question - if I wanted to impose the new settings on a virgin system, what would I do ?
Would an export/import of DeviceSettings and a save/load of MachineSettings be enough ?
Okay good. I was reviewing the thread and noticed one thing.
The “S-Value max” setting in Edit->Device Settings is currently set to 10000 but needs to match this value. Change S-value max to 255. This will directly affect power modulation.
I assume you mean for the same system. Ultimately there were 3 meaningful changes that were made:
G10 L2 P1 X-400Y-300- This is the work offset that defined your origin. This would not get picked up in Device Settings or Machine Settings backup so you’d need to apply it$10=0- This changes GRBL configuration to report status to work position rather than machine position. This would be preserved in Machine Settings backup- S-Value Max to 255 - This sets upper bound value for power modulation. This would be preserved in Device Settings .lbdev backup.
OK. S-Value max set.
I think we are good. Thanks very much for your help and patience.
And, Happy Holidays !!
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.