How to set up Tool Offset in MACH2?

[High Seas]

Here's something I could use some help on.
How do you set up tool offset?
Here is what I've done so far - read the book - Yep
Searched here and Yahoo - Yep.

And, I have set up a tool in the Tool Table, given it: a name, a diameter, z offset (0) material, etc.
Used the ENTER key and even Saved the Table.
Selected the Tool Number, and then went to the Offsets Tab (ALT5).
Checked that I had the tool number selected and the diameter was the same.

BUT THEN, I note the Program Extrema (on ToolPath Alt4) doesn't change indicating the offset is there!

I've been playing with the wizards for circle cutting. When I use the wizard and change the offsets, the Program Extrema DO change - reflecting the change in offset.

I note that an M code is in the code when I use the wizard. I checked it and its for a tool change. Is that what sets the offset? I want to set offset in MACH2, not the cad file.

Help!!!! What step am I missing? Is there something I need to do in config?

ANYbody? TIA - Jim

[Al_The_Man]

Does the mach 2 accept G41 G42 to implement the tool offsets?
Al

[HomeCNC]

Here is the way I use tool offsets with Mach 2 on my jobs. (I also use fixture offsets in combination with it)

In order to fully use tool offsets you need to use fixed collets to hold your tools. The mills are clamped into the holder by some means like a set screw. This keeps the tool at the same place when the collet seats in the spindle.

First you need to record the length of all your tools. My example will be with my CNC router and my Porter Cable router with my fixed tooling. I move the Z axis (with no tool) down until I just touch the spindle on the table. If you can't go that far down with no tool then use some spacer blocks under the spindle to raise the surface up. when you just touch this surface you need to zero the axis manualy. Raise the Z axis and place your first tool in the spindle. Move back down until you just touch and read the axis readout for Z. This is the length of that tool. Enter this length in the tool offset database in Mach 2. Do this with all your tools.

To begin the job I home the machine so my X=0, Y=0, & Z=0 at the far end of my table. I move the tool to the corner of my part and note the X, & Y readout. I enter this data in the fixture offset #1 for X and Y. Now I remove any tools and lower the Z axis to touch the spindle on the material top. I record this number in the fixture offset for Z distance.

In order to use the fixture offset and tool offset in Gcode I need to make sure that I have the proper code for them in the file. A G54 will use fixture offset #1 and a G43 T# will use the offset for that tool #.

You should see the DRO change when you activate the offsets. If you instruct the tool to move to 0,0,0 you should be at the corner of your material and just touching the top of the material with the tool in the spindle.

[High Seas]

Al_The_Man.
Yes it seems that MACH2 does take G41 and G42. But as I read them they are: Cutter Compensation LEFT and RiIGHT. So do I input a line in the GCOde for each pass, so the compensation is on both sides? Or does machine code then figure out to go in al directions and just the initial compensation is Left or Right?

HomeCNC,
I'm working through your approach. I'm not there yet. Figuring out fixtures etc.
As I read the G43, that is Tool Length compensation - and so far I'm doing all that manually. I was wondering the same as I responded to Al - is there an easier way? Suppose I could "scale up the X and Y axis to compensatefor the cutter?

Thanks for the tips guys- but I'm still scratching my head and looking!
Thanks - Jim

[Al_The_Man]

The G code offsets are usually modal, i.e. the remain in effect after you issue them until cancelled by a G40 etc, so you do not have to issue them for every line of motion.
The side that is offset (left or right) is as you are looking at the cutter from the rear, behind the motion of travel. With most systems you have to have a pre or dummy move at the issue of the first G41/42 into the cut that is greater than the dia of the tool, it then takes effect for every move after that until cancelled. Obviously the purpose of the tool offsets is that you program the part as exact size and the tool is moved over for its radius.
Al

[ger21]

Originally Posted by High Seas Al_The_Man. Yes it seems that MACH2 does take G41 and G42. But as I read them they are: Cutter Compensation LEFT and RiIGHT. So do I input a line in the GCOde for each pass, so the compensation is on both sides? Or does machine code then figure out to go in al directions and just the initial compensation is Left or Right?

Jim, you only need one G41 or G42, and one G40 at the end of the cut to turn it back off. I haven't used Mach2, but here's how I do it. Say you're cutting out a square, cutting counterclockwise (conventional milling). You usually need to add a start segment for the tool to have a chance to offset before you actually start cutting your part. So, Starting from the lower right corner of a 2" square:

G0 X2 Y-2.5 (Move a little below the corner to allow for the offset to happen)
G1 Z-.25 (Whatever depth you want to be at)
G42 (offset to the right, because we're cutting counterclockwise)
G1 X2 Y-2 (The offset should occur during this move, the bottom corner of our square)
G1 X2 Y0
G1 X0 Y0
G1 X0 Y-2
G1 X2 Y2
G40 (Turn off comp)
G1 X2.5 Y2 (Run a little past the part, while the tool moves from the comp'ed path back to it's actual path)


This is how G41 G42 operates on our router at work. I'd expect Mach2 to be similar. The manual is a bit confusing on Cutter Comp. I pointed this out on the Yahoo list so hopefully it will be better documented in the future.

[HogDog]

Check out Mach 2, Manual Automatic Tool Change parts 1-3 at industrial hobbies

[High Seas]

Getting smarter by the minute! Thanks Guys - I'll go give it all a try!
YES! DON'T FORGET TO HIT THE 'Touch Button"! Doooh!
Cheers - Jim