G-Code G28 Return home:
G28 Is the G-Code that instructs the Controller of the machine to move the tool automatically to the reference point. The Reference point is the fixed position on the machine, to which the tool can be moved. This reference point is also called the “Home position”. Machine has the reference point for X, Y and Z Axis.G28 G-Code Format:
N170 G90 G28 X_ Y_ Z_; (Absolute Code)Or
N170 G91 G28 X_ Y_ Z_; (Incremental Code)
Where X, Y and Z can be used to indicate an intermediate point, through which the tool will pass, before continuing to the reference point. If the intermediate point is not set, tool may move in non-vector type path. It may collide with the part or the fixture, so you can put the intermediate values in X, Y and Z to move the tool first to safety plane.
The move to any intermediate point and the reference point are performed at a rapid traverse rate.
Example Below shows the collision scenario 1:
The diagram below shows how the tool could collide with the billet when moving towards the reference point with Non-vector type movement.
To avoid this collision, the tool is sent on a path which includes intermediate point P2. The intermediate point is used to allow the tool to move completely clear from the billet, before continuing onto the reference point, P3.
The above tool path can be programmed as follows (In absolute mode, G9Ø):
G90 G28 X60 Z60;
The above tool path can be programmed as follows (In incremental mode, G91):
G91 G28 X0 Z40;
So that the Tool moves to the safety plane before it reaches the Reference Point.
Example Below shows the collision scenario 2:
In the diagram below, the tool is in a position (P1) where there is no obstacle to collide. The intermediate point, in this case, is not required, so the block can be written as follows:
(In incremental mode, G91): G91 G28 X0 Y0 Z0;
