Replacing elderly Anilam 1100 control system on vertical mill

[Muzzer]

My Acorn system allows several G28 / G30 "return" positions to be stored, for things like tool change, tool setter, park etc. But G28 seems to be quite a confusing command and is interpreted and implemented differently depending where you look. I don't recall a similar table of return positions in the Newker controller.

There's the option to set coordinates for the electronic tool setter in mine. As I have bolted mine to the table, I use that option. The alternative is to simply sit it on the table under the tool. The advantage of that approach is that you can also use the tool setter to acquire the top of the stock, by sitting the setter on top of the stock, touching off, then automatically subtracting the height of the setter from the Z coordinate.

There is an MPG input on mine which I use with a wired MPG but I looked into using the original DRO linear encoder inputs to display actual position rather than commanded position. Thought that sounded like a nice idea - I'd come to believe this was possible but turns out it isn't. I could still use an index pulse output from the motor servo drive (if it was available) to improve the homing accuracy but on my Bridgeport that would be lipstick on a pig.

If you want to use the handwheels and see where the machine is, I think you'd need to have the "absolute" version of the controller which communicates with the servos through some sort of serial bus. Even then it's not clear if that mode is supported.

[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.