I’m using Fusion 360 and the Easel post processor. The nc file produced does not contain a G28 and I am unable to find any settings to turn it on.
Does Easel inject this in when you carve with the loaded g-code?
No. Can you explain why you want the G28?
EDIT: Easel adds a G28 for the Carvey, but for some reason, I assumed X-Carve.
Using the same concept of the Carvey, i’ve mounted a squaring block on the wasteboard so my starting point is alway the bottom left of any board. The first thing I do when turning the machine on is to home, move to predetermined location of the bottom left corner. Then use the Z-probe to set the height, followed by setting the G28 location. This is all done by issuing one script. If the g-code file has a G28 in it, I can carve multiple times and/or multiple files without having to worry about manually issuing G28 again. It’s easy enough to add to the file by hand but old post indicates it should put it in.
BTW in case you are wondering about my possibly hitting clamps etc, I use clamps that clamp from the top and right side pushing back to the squaring block. The hight of these clamps are lower than the surface of the of the carving board. At least in my case, if I were to carve something less than 3/4’s then I would have to use different clamps.
Does your G28 location become your Work XY zero?
In most cases I’ve seen on the forum, the G28 is an extra, unnecessary step.
G28 is primarely a “parking spot” and set once (untill you want to assign the parking to a different spot. Its function is not related to work zero or as a reference point.
Work zero is stored between power cycles so if coupled with homing switches you can have a fixed work zero reference without using G28.
Typical workflow, initial:
- Perform a homing cycle (Homing switches provide a machine-workspace syncronization)
- Jog the bit to your work zero position
- Confirm “Home position”
- Carve
After a power cycle:
- Perform a homing cycle
- Reset Z
- Carve using “Previous home”
So if you want to carve multiple identical jobs simply remove done material, insert fresh and carve again, this time clicking “Use previous home position” in Easel.
And if you for some reason power down the CNC you can keep using the same work zero provided you Home first.
I think you miss my point here just a little bit. I’m trying not to have to JOG at all, ever. Actually I am doing it now, I just have to insert the G28 myself. Again the old posts for easel post processor says to select it in options but it’s not in the current versions. The Fusion 360 post processor has the option.
There has been a lot of miss understanding about G28 and how to use it. Many don’t understand the machines path to it so it historically has cased people to crash into clamps, etc. I suspect it was removed to cut down on customer service issues, but don’t know that.
Now with that being said, I have tried several times to tell easel to use last home and it does not seem to work for me. I think the X&Y worked fine but the Z did not, but I don’t really remember. I just know I give up on trying to use it. Could be user error on my part for sure.
I do not understand your reasoning for adding G28 into your work flow or assigning G28 each time (I am no expert so I miss your intent) Can you elaborate on that?
Trying to eliminate manual jogging I can understand but where G28 fit in your workflow I miss out on 
In Easel - using “Use previous Home Position” X/Y is given but Z need to be reset in case you have changed tool with shorter/longer tool stick-out.
So to me, a practical workflow would be something in the line of:
- Home the machine
- Move to predefined G28 (or G30) located above a fixed Z probe
- Probe Z to reset tool height
- Easily handled by a script
CNC is now ready to carve, work zero is remembered from last carve, or you re-assign if different from last.
G28 (or G30) do not need to be re-assigned between carves (unless you want the parking spot to change relative to machine coordinates)
1 Like
A G28 command just moves to your G28 position (set by sending the command G28.1 while at that position). The G30 command works the same.
Having your machine automatically go to G28 before it carves does not set any zeroes. The machine will go to G28 and then carve based on wherever your WCS (Work Coordinate System) origin is.
All “Use previous Home Position” does is NOT send a command to set the XY origin. Your machine will automatically use the previous WCS offset…it has to. If you don’t want to set Z each time, you can always use a different sender. Once your XYZ WCS origin is set, just home and carve. I do this frequently when I don’t need to be cautious about my Z height.
I use G28 for a tool changing location and G30 for a “get out of the way, so I can work” position.
1 Like
Ok, Maybe I misunderstand it’s use. Maybe someone can explain the following to me. What is the purpose of the G28 code inserted by the grbl post processor.
Below are excerpts from the different post processors.
The easel one, the grbl one with G28 options turned on, and the grbl one with G28 options turned off.
Easel Post Processor
====== Start Code=======
G90G94 ( G90:Absolute prog G94:Inch per minute )
G17 ( G17:X-Y plane selection )
G20 ( G20:Inch system selection )
======End Code======
G0Z0.4 ( G00:Rapid positioning )
Grbl Post Processor with G28 Option
====== Start Code=======
% ( %: Start or end of program )
(1001)
(T1 D=0.125 CR=0 - ZMIN=-0.75 - flat end mill)
G90 G94 ( G90:Absolute prog G94:Inch per minute )
G17 ( G17:X-Y plane selection )
G20 ( G20:Inch system selection )
G28 G91 Z0 ( G28:Return to home G91:Incremental programming )
G90 ( G90:Absolute prog )
======End Code======
G0 Z0.4 ( G00:Rapid positioning )
G28 G91 Z0 ( G28:Return to home G91:Incremental programming )
G90 ( G90:Absolute prog )
G28 G91 X0 Y0 ( G28:Return to home G91:Incremental programming )
G90 ( G90:Absolute prog )
M30 ( M30:End program…rewind stop )
% ( %: Start or end of program )
Grbl Post Processor without G28 Option
====== Start Code=======
% ( %: Start or end of program )
(1001)
(T1 D=0.125 CR=0 - ZMIN=-0.75 - flat end mill)
G90 G94 ( G90:Absolute prog G94:Inch per minute )
G17 ( G17:X-Y plane selection )
G20 ( G20:Inch system selection )
======End Code======
G0 Z0.4 ( G00:Rapid positioning )
M30 ( M30:End program…rewind stop )
% ( %: Start or end of program )
I said I was using the easel post processor, not easel. My g-code is being sent via universal g-code sender. There is not last used home that I am aware of in it.
Moves only Z axis to wherever you set your G28.
Moves X&Y to wherever you set your G28
The G91 with them makes the zero a non move rather than moving to X0Y0 before moving to the G28 position. By specifying the axes, the machine will only move those axes.
Your zero doesn’t change unless you change it. If you power on, home, and start a carve, it will use your same WCS zero that had been previously set.
“Use previous home” is Easel speak for using the previous work zero over again. Since work zero is an offset to machine zero previous work zero is known.
In UGS, for the 2nd carve from a known work zero after power-up simply home the machine, open file ( and reset Z if different) and hit run. G28 is not a prerequisite at all.
G28 (and G30) is an arbitrary point within the CNC work space and stored as an offset to machine home, which is not linked to anything related to work zero.
G28 and G30 for our hobby machines explained:
