We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that youāve provided to them or that theyāve collected from your use of their services. Learn more.
The reason I use G53 in the post-processor is to lift the spindle in machine coordinates : whatever your work-coordinates settings, the spindle will go up to the maximum z-axis.
If after homing you are at 0,0,0 (with the spindle up), then G53 G0 Z0 will lift the spindle to this home z -position.
Typically GRBL stays a few mm away from machine 0,0,0 in order to not cause false limit switch triggers.
So if your machine home is 0,0,0, and you stay 10mm safe, then your safe home position is -10,-10,-10
@Strooom I donāt think @KikoLobo is using your post processor. Wouldnāt he raise Z and THEN move XY if that was the case? The error he did a screen capture of is not due to the G54, although it appears that way. He probably has an M6 on the preceding line which throws that error in cncjs.
So yes, I am using @Strooom pre-processor in Fusion360. I think my mistake is using the easel pre-processor and not the OpenbuildsGRBL oneā¦ In the repository it comes with two files. I am using: f360-easel.cps ā¦ Will try OpenBuildsGRBL.cps instead.
Here is the first section in the .nc file. As can see in the screenshot thereās both G54 and M8T1 near line 9 [where the controller reports the error]. If the error comes from M8T1, then the error is not the causing issue of the movement beyond the end stop in the Z Axis.
I am switching to OpenBuildsGRBL Pre-Processor. Will let you know if issue persists.
@KikoLobo
Machine coordinates:
Z0 = your limit switch / home
Z-7.4ish = your work 0 / top of work piece
Thatās a difference of 7.4mm. Your gcode is telling the spindle to lift 15mm.
Not enough room.
Is this a post-processor issue? Or a cam job setting issue issue?
The work area is big enough for the job, itās just that command that rises the bit more than it should. It might be the job settings in Fusion360 for the carve.
No problem. Again, use default grbl post, and share your Fusion file if you have more questions. With just over 7mm of clearance over your stock, youāll need to pay close attention to your CAM settings.
The Z-15 command is lowering the tool -15 mm below Z0. This is not lifting the tool as you wrote, this is lowering the tool.
So all the time Iām home my x,y,z to the left bottomposition and scratching the tool to the material surface, I zero all axis and send a G28.1 for a new material homing.
The generated g-code (actual openbuildGRBL from the git hub) is trying to āliftā the spindle up with:
G53 G0 Z-10
G54
But this command is lowering the spindle about 10mm into my material. Crash!!!
Iām using GRBL 1.1 on my chinese ācheeseā mill Genmitsu 3018-pro.
Is this the wrong post processor or can I change this behavior?
This move will move the spindle to 10mm below MACHINE zero? It is intended for use with homing switches. Use a different post or edit that one.
G28 is pretty useless without homing switches as well.
No, G28.1 creates a G28 position which could be used for any number of reasons. A WCS zero is set with a G92 (temporary) or G10L20 (persistent). Without homing switches, it all needs to be reset every power cycle.
Not true, if my spindle is at Z-20 a move to Z-15 is a move up.
Without homing switches, your machine position is arbitrary. Donāt use it in commands.
G0 Z-10 is a standalone command that could have different results.
If the motion mode is absolute:
If there is a G53 preceding it, on the same line, it is a move to MACHINE Z-10. (could be up)
Otherwise it is a move to WCS Z-10. (could be up)
If the motion mode is incremental:
It will move the Z down 10 from where it is.
Hi Neil,
Sure if you at negativ 20 a Z-15 will move the spindle upwards.
But we are talking about to set the home position of our material, which is here at the left bottom if you look from top to the x,y axies.
Then I have to lower my z axies till the tool is scratching the surface.
In GRBL 1.1 is re-setting the x,y,z position to zero of all three axies by using this G28.1 - that is how it is working.
From this position I need to run the g-code, but the postcontroller always writing this Z-15 at a very first command which is not lifting the spindle.
As a GRBL G-CODE it needs to lift the spindle about 2 mm which would be a Z2 command and move the xy to the start position.
This is the whole issue here with my mill, and I still wonder in accordance of the postprocessor description, that the Z-15 command should lift the spindle, but -15 is a command to move it down.
