Replacing elderly Anilam 1100 control system on vertical mill

[JAZZCNC]

In the Fanuc standard G28 and G30 are actually simple commands but easily miss understood and used. How G30 works also depend on the controller.

G28 just returns to MACHINE zero, however it does this by way of going thru an intermediate point first, or it can if required. Also how it works changes depending on G90, G91 modes and it''s this that I think catches people out most.

For instance in theory you could just type G28 and nothing else and the machine would go to the MACHINE ZERO position, however, the Fanuc standard requires you enter an Axis and a value, this value is the intermediate position the axis should go thru on it's way to MACHINE ZERO.
In practice, the current Position the tool is located is often used for the intermediate value and the Axis then goes straight to ZERO. But here is where it can get funky, this depends on what mode you are in G90 or G91. For instance, these two example lines below will give exactly the same movement. For this example assume the tool is located at X10.
#1
G90
G28 X10

#2
G91
G28 X0
Both these commands will move to the MACHINE ZERO via the intermediate point.?

With Example, #1 X10 is the intermediate point, which is the location of the tool now so it goes straight to MACHINE ZERO.
But with the example, #2 things are different because we are now in the INCREMENTAL mode so we are no longer going thru an intermediate point but rather moving an intermediate distance on the way to ZERO. So X0 is seen as moving zero distance and then the axis goes to MACHINE ZERO.
Now if the code read as below it would be different again.
G91
G28 X10
In this case, the X-axis would move 10mm positive from its current location then move to MACHINE ZERO.

Now G30 is actually classed as a move to a secondary ZERO position and depending on the controller can actually have several ZERO positions.
But again in practice, it gets used exactly like G28 because of how it works.
G30 works just like G28 and sends the Axis to ZERO by going through an intermediate position but G30 works by going to the secondary ZERO which is set in the controller parameters. Depending on the controller you can have several G30 ZERO positions that are stored in parameters and called by using a "P" address.
So G30 P3 X10 would move to or thru intermediate point X10 then use the value stored in parameter #3 and move the X to this ZERO location.

However, often just G30 X10 would be used and in this case, because no "P" address is given it assumes "P1" as a default ZERO value and because many people don't program the Controllers Secondary ZERO position or the controller doesn't have this option then G30 is used just like G28 and sends the axis to ZERO.

But in essence, both G28 and G30 simply just move to MACHINE ZERO via an intermediate point.