How to manually set the z axis

1

I am trying to set the home condition as follows (X AND Y TO 0, Z TO 1 INCH). The file that I am using the first cut should be less than .20 inches from 1" to .82". When the Z axis is set to zero, the first cut is like 3/4".

2

wow so much info/details missing… Not sure how to help? System you are using, software, etc?

3

Hey William,

driving Z to “1” inch is not possible since Z travel goes from 0 to −133 mm (0 to −166 mm with Z-20 “heavy” slider). I assume you mean 1 inch above the worksurface. This value is not known as it differs strongly between the machines, depending on your setup of wasteboard etc., you got to probe it.

To move to X=0 and Y=0 first, you could enter this into your manual data interface (MDI):

G20 ; Set imperial units mode
G90 ; Set absolute distance mode
G53 G0 X0 Y0 Z0; Rapidly move to the machine's home position in machine coordinates
G92 X0 Y0; Set the X,Y posistion as the new zero coordinate of the new coordinate system in effect

G92 is the most important command in a probing sequence, you could also simply probe XY instead of G92. Note that this is somewhat superfluous since X=0 Y=0 is the machine home and is already the zero coordinate in the default coordinate system. But it drives Z to its highest (zero) position.

Now you could lower Z by probing (comments including the “;” are ignored, can be pasted or omitted):

S0 ; set milling motor speed to 0
G70 ; Save all modal modes
G21 ; set metric mode
G0 Z-80 ; Lower Z to a position -80 mm
M0 (MSG, Please connect the touch plate to the controller, place the touch plate underneath the bit and attach the magnet end to the collet of your milling motor.) 
F100 ; Set feedrate to 100 mm/min for probing. (which means slow) 
G91 ; Set incremental distance mode 
G38.2 Z-90 ; Move the milling motor downwards until the bit touches the touch plate 
G92 Z15.4 ; Set this position as the new Z zero value (to reflect new tool length - including subtraction of the touch plate's height which is 15.4 mm thick) 
G0 Z30 ; Lift Z by 30 mm 
M0 (MSG, Please remove the touch plate and start the milling motor)
G72 ; Restore all modal modes that were saved previously

Now you have set the Z zero to the machine workbed.

(You could also simply press the “Z probe” button instead of entering all these commands.)

If you then want to move 1 inch above workbed, you enter:

G20 ; Set imperial units mode
G91 ; Set incremental distance mode
G0 Z1 ; move upwards 1 inch
G92 Z0 ; set this z heigt as the new zero coordinate.

See also

With your gamepad, or with the Jog Pane, or with MDI commands, you must move the bit closely over the circle in the touch plate prior to start probing.

See also

1 Like
4

HOME position is always going to be X0, Y0, and Z0, where X and Y are at full negative travel limits, and Z is fully at the top of its travel limit (fully + travel). I believe you are adding confusion by trying to use HOME position rather than a WCS (workpiece coordinate system). Home is merely a known position for machine reference. This is a repeatable location that is also used for reference to machine travel soft limits.

For any project, you should be using a WCS. The normal workflow would be to set this per your workpiece and how its programmed, then use your probe to set Z zero to the top of your workpiece. Then, any work-engaging Z moves will be in the Z- direction.

Your machine should be pre-programmed with a Z ‘safety height’. This is an imaginary plane set above your WCS Z zero. I’m not sure what this dimension is on the 1F controller. I run a different controller system, and mine is typically set at .2" (5.08mm) above Z zero. So whenever the machine is making a jog move (a non-cut move), the tip of the cutter always retracts to the Z safety plane.

2 Likes
5

Hey Bill, hey all,

another word that I saw frequently used is “origin”, like “workpiece origin” for “workiece zero coordinate” or “machine origin” for “machine zero coordinate”.

The buildbotics-derived Onefinity controller has no setting like this, but of course you can program a safe height in the toolpath.

What you can use is G28 (Go to a predefined position):

G28 Z-40

In this example Z=-40 mm is the “safe height”. The command will first go to Z-40, and then if nothing is set in #5161–#5163, go to machine home. If you want it to go to another final position you got to write values into #5161–#5163 for target X,Y and Z.

Useful for going to home position if you are at the bottom of a pocket :slight_smile:

(Note: Does not work with the Masso, as the Masso g-code lacks the parameters and G28 is not used the standard g-code way).

1 Like
6

Hey Aiph5u,

Yes, this is quite correct, I totally mis-spoke in saying that was a function of the controller. It’s not, it’s a function of the g-code which is set in my Estlcam software. Not sure what I was thinking… :roll_eyes:

Also correct on the other terminologies you listed, such as ‘origin’ and ‘workpiece origin’. It’s very important to understand and distinguish between this, and the ‘machine coordinate’.

2 Likes