Question about Referencing and Zeroing.

[redbaron]

I have a gantry router with a home position (0,0,0) at the lower left of the table with the router positioned at the top of the Z-Axis. My table has an offset of about -6.5" which then sets the Z offset to +6.5.

My Question is that every time a program initializes or I want to put the tool at a fixture offset, Mach 2 trys to raise the tool by it's own length before lowering it to 0. This really is noticable on my fixtures which are taller. There is plenty of room (+1") between my longest tool and the top of the stock, but Mach2 is trying to raise the tool by it's tool length (ex. 1.6") before lowering it to 0 or safe-z. This of course triggers my home/limit switch because it is less than the length of the tool.

I have set the safe-z to 0 and this does not fix it. Is there a way that Mach2 2 can just move to X0,Y0 and then lower to Z0 without raising by a tool length before doing so?

Am I making sense? Am I an idiot!?

TIA

[redbaron]

This might help. I'm not sure it's a Mach2 thing or not but her is my init G-Code.

N10 G20
N20 G0 G17 G40 G49 G80 G90
N30 G64(CONSTANT CONTOUR ON OR TURN OFF W/G61)
N40 (2 1/2 Axis Pocketing)
N50 T2 M6
N60 G43 0
N70 S10000 M03
N80 G00 Z0.7500

[HuFlungDung]

I'm not sure if this is part of your problem but your line:
G43 0
looks a little suspect.

The G43 command is the length offset command. Typically, it should be followed with a "H" address and a number corresponding to the correct entry line in the offset table:
G43 H2
would be a typical example. The value associated with "H2" would be the Z length offset for that tool 2.

I don't know anything about how Mach2 works, but there may be a setting where you can tell it to add the tool offset movement into the next Z movement. This would eliminate the movement caused by simply calling the tool offset. Might be worth a look.

Other that that, I can describe a method I developed on my old Bandits, which always executed a movement for every tool offset call: Call the top of your work Z0. Or even better, use some kind of a standard guage to set your tool lengths to, something that would typically be above your part's Z0.

I always began the tool setup by measuring the offset of the longest tool first. This would help me judge how high my "guage" would be. I always wanted my offsets to be zero or negative values. Thus, when they executed, the tool would never rise and hit the limit.

Once all your tools are set, you can measure the difference in distance between your setup guage and the top of the part. Do this in jog mode perhaps, zeroing on top of the guage, and then jogging down until you touch the part, with a paper feeler guage to help you sense the touch.

Take this measurement and enter it into the G54 work offset table Z column, which I'll assume Mach2 also has somewhere.

Near the beginning of your program, you will want to call for the G54 work coordinate system before any movements are made. You use the X and Y values in the G54 to determine how to get your tool from home, over to the reference corner of your part anyways. So now, you also make use of the Z value in the G54.

What you should then see is this: you call the tool change and call its length offset. The tool moves down so its tip is at the height of your setup guage. Then, you set the machine into the G54 work coordinate system, simply by placing a G54 in your program.

Now, when you call for a Z1.0, the tool should move to a height of 1" above your part's Z0.

[redbaron]

Thanks mucho for the advice. I'll take a look at the G43 command and see if that's the culprit