Using tool offsets on a Bandit

[Chris64]

Has anyone done this? I've avoided it so far by doing my own math, but I am finding that it would be nice if I could just specify the tool and it would handle the offsets appropriately. The manual does a good job of confusing me. I don't understand when it says right offset or left offset...which way is left? I know this seems obvious but what if I'm cutting just on the X axis? What would it do then? Corners are whole other story.

My initial preference was just to program the offsets myself so there are no surprises. Well, it sure would be nice to be able to rough, finish & chamfer all from one program rather then having to write three seperate programs.

Thanks

[Geof]

Most manuals are very good at confusing. Left or right offset? With left offset the centerline of the cutter is following a path which is to the left of the cut line. With a cutter rotating clockwise this is climb milling. Right offset is the opposite and that is conventional milling. Doesn't matter what axis you are cutting on; for interpolating a circle with left offset and G02 the cutter centerline is going around the outside of the circle and with G03 is going around the inside of the circle.

[HuFlungDung]

Chris,
I forget the exact revision of your Bandit firmware. Are you quite certain that it has the capability?

To get into the length offsets register, in MDI you hit
/T START
The command window shows a single digit which represents the address of the register.

Similarly, the tool comp register is accessed in MDI by typing
/N START
Enter a radius value and hit STORE to store it. Remember which address you used for which radius.

Now if your firmware has the capability, you need to use a 5 or six digit tool number when you call the tool offset and wish to use radius compensation, as opposed to the 3 or 4 digit number used when your only interest is calling a length offset.

The manual may show you the 6 digit number in this format:
Trroott
where
rr is the radius comp register address
oo is the length offset register address
tt is the tool number to be applied to.

To keep it all simple, lets say you use radius comp address 1, length offset address 1 for tool 1. The six digit format is
T010101
The Bandit drops the leading zero I think so it will look like this for single digit addresses:
T10101

You may also mix and match comp address and length offset addresses to suit your own purposes. That is for advanced use. You might want to 'permanently' enter certain common tool radii in certain fixed comp addresses and then you would always know which one to call by maintaining a chart of the values.

So you call that number whenever you first call up a given tool. Then, whenever you are ready to apply radius comp, all you have to do is put a G41 or a G42 in your program, on a line all by itself. The moves that follow will then be radius compensated by the amount that you entered in the rad comp register (radial values only, IIRC).

Bandit is not really smart. So when tool comp is activated, the control will most likely jog the tool in some random direction (along one quadrant line) by the full amount of the radius comp value that you used. Compare this to newer controls that do not move the tool until the first feed move is encountered at which time the comp is applied.

So, start your tool at a safe distance from the part profile so you don't get a gouge. As per usual, you need to add a lead in and a lead out segment to your part profile, to allow the cutter to shift position. In the case of the Bandit, it needs to see a feed command so that it knows which side of the line is left and which is right. The control has no lookahead.

Be sure to cancel the compensated path with a G40 when you are done, as G41 and G42 are modal. It is a good idea to program a G40 at the beginning of every program, in case you abort while radius compensation is still active.

[Chris64]

Wow, that's informative...in a familiarly confusing way. I think I probably just need to monkey around with it a tad.

I'm not sure if my system supports it. I believe the firmware is 2M, but so far all the commands in the manual seem to work so I assumed that this one would too.

Eitherway, would it be considered acceptable/normal to handle the compensation manually? I've been working on a program to simplify the coding. It could easily manage the tool offsets but it's not as efficient with memory usage. For example; It would require nearly 3 times the code if there were 3 tools used (as opposed to a single set of commands repeated with just a tool change).

I'll play around with it a little so I can get a feel for it (and do determine if I actually have it).

[Chris64]

Oh yea, and thanks for all the details. I really appreciate it.

[HuFlungDung]

Chris,
According to a chart I have, level 2M firmware does not have the capability. For that you need the 3M.
If you contact Albright CNC, I'd be surprised if he wouldn't burn you a new EPROM to bring the thing up to the highest level. Tell him you're thinking of getting a Shadow, so you can get a good deal on the chip My bad