G28 will simply move to the previously defined G28 location, in one, straight line motion. As I’ve said, it’ll move X,Y, & Z together and caution should be taken.
You can use intermediate points with G28.
Let’s say my end mill is at X150 Y80 Z3, and my G28 location is X0 Y0 Z50. I can specify an intermediate point when using G28 to make my Z move straight up.
G28 X150 Y80 Z50 will move my end mill to X150 Y80 Z50 before continuing to X0 Y0 Z50
If you don’t specify an X & Y it will only move the Z, and not continue on to X0 Y0.
G28 Z50 will just raise your Z. Follow that with a G28 and you’re right where you want without crashing.
Another way would be to use G53 Z-10 to raise your Z to 10mm (I’m assuming mm) below the Z limit. Then use G28.
Here from the horses mouth in case someone wants to verify the info:
What about G28 and G30?
G28 and G30 are not WCS settings.
G28 and G30 are persistent, stored positions that you can send the machine to with a single command. G28.1 and G30.1 are used to store the current machine position in absolute machine coordinates.
You set the G28 position by moving the machine to the position you wish to set and issuing G28.1. G30 is set the same way, but with G30.1. These commands do not take any values, and in v0.9 and possibly v0.8c of Grbl, passing a value will cause the machine to move.
Once they are set, you can issue the G28 or G30 command and the machine will move all three axis, at rapid speed , to the predefined position. This behavior can be changed w/ using suitable commands in versions of Grbl which support the additional inputs.1
Note: These commands will not raise the Z axis before moving the X and Y so use caution.
You can specify an optional, intermediate position by adding X, Y or Z values to the command.
Important Note: These coordinates are in the current WCS, not absolute machine values.
So if you wanted to raise the Z first, you could say G28 Z1.5 and it would rapid the Z to 1.5 - in the current WCS - and then rapid move X, Y and Z to the saved position.
Yes, that is the correct answer that should have been posted 
to avoid some newb form getting hurt.
…
Tonight I tested the G28.1 and G28… and it worked great!
From your guys posts I was aware that G28.1 also stores the current Z position, therefore I made sure to keep the bit in up position when I sent the code. I always re-do Z-Zero anyways when I start a new job or flip a piece. After sending the G28.1 code I did several tests, including making new XY zero points and turn the machine off/on… Then sent the G28 and tested the CNC recalled position by running my previous job on same wood piece that I had milled before and it ran the path without widening any previous groves.
UPDATE: I had noticed a strange behavior in the Carbide Motion build 513 software, but because my problem went away I thought I had just typed something wrong… Now I am convinced there is a BUG in my version of the software. If I enter code (like /G28) on the MDI page, then on the Jog page press ANY manual move button, then the machine just takes off and does not stop until it is at the last used rapid stop position. Does anyone else have this problem?.. What is the latest version of the CM software?
Btw: I can work around this by sending the code twice… Example: I type /G28, then wait until the machine is in position, then hit enter to send the /G28 again… after that manual buttons on the Jog page work normally again…
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.