Re: power up and homing
None of the bandits I ran (3 out of 3) had any provision for homing. G99 was the return to home command. If they would have this option turned on, it would have been merely to a switch anyways, which would not be particularly accurate. I always used the mechanical dials on the screws to keep track of the home position, and would carefully park it at shutdown and make sure to reset the mechanical dials to zero. Often, the drives would pulse a bit on powerup, so you'd have to watch for that occurance.
So when the control powers up, all axis are zero. If you want to move it somewhere and set a new home zero, then you can do so using the G92 command. You can set any value you like with the G92, but if you want all zero then:
X0 ENTER Y0 ENTER Z0 ENTER G92 STORE
You can also do a single axis at a time.
G98 START (in mdi) will send all axis home to the set G92 position.
All the Bandits I've seen used a seperate 110v supply for the Bandit. The reason for this is preserving the program in memory requires constant power. The Standby switch on the Bandit keeps the memory alive and keeps the boards warmed up. So the main disconnect for your 3 phase is handy as a seperate unit so you can shut down the axis drives (if they are hooked up elsewhere to power, although the Bandit sometimes had power supplies for the drives built in) and kill main power to the machine and toolchanger.
If your Bandit has axis displays, then you can reset them to whatever you want them to read using the G93 command and setting commands in mdi just as you would for G92. G93 is display control.
T1 M6 should invoke a tool change, but will not call the length offset. So you could first change the tool, then farther down in your program you could implement the length offset. Because the Bandit executes the length offset as soon as it is called, you would want to do this when it was appropriate and safe to do so.
The Bandit had a strange coding method for tool length offsets and radius comp.
You could use T1000 as a means to call the length offset for T10, or T100 for T1.
If you also planned to use radius comp, then the number became T101010 where the secret code was related to this acronym:
Trroott
rr= rad comp number
oo = length offset number
tt = tool number
So you could use two, four or six digit command, and a leading zero would be dropped so that T010101 = T10101 for T1
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)