[ckirchen]

To overcome the limitations of G43 (axis moves by itself and actual Z coordinate is not shown), I wrote myself a macro that modifies the G55 work offset by the tool offset (I use a single WO for most of my work). So, instead of commmanding G43H02, I command M98P9043H02.

The macro has been working well up until today when I had to modify it to change all of the work offsets at once (G55 to G59). All of them change like they should (WO_new = WO_old + TO), except for G57. Instead, it does WO_new = WO_old + 0.1 * TO. I found out the hard way; the tool holder plunged into the fixture on the station corresponding to G57. Fortunately, it was a plastic fixture and the spindle tripped pretty quickly, so other than a big gouge, there was no real damage done.

I modified the macro to include a 10x multiplier, but I feel extremely uneasy in doing so. Is there a parameter that controls this? The machine use inches and metric (currently set for inches), but the manual shows several metric specs that are 10 times the inch number (i.e. it lists .001mm/.0001" as the minimum increments). My thought is that there is a parameter for G57 that didn't get changed.

Here's the macro:
%
O9043
(G43 - TOOL LENGTH SET)

(CANCEL CURRENT OFFSET)
#2702=#2702-#501 (G55)
#2703=#2703-#501 (G56)
#2704=#2704-#501*10 (G57)
#2705=#2705-#501 (G58)
#2706=#2706-#501 (G59)
#500=1 (RESET TOOL NUMBER)
#501=0 (RESET OFFSET VALUE)

(APPLY NEW OFFSET)
#500=#4111 (GET TOOL NUMBER FROM COMMAND)
#501=#[2000+#500] (RETRIEVE OFFSET)
#2702=#2702+#501 (G55)
#2703=#2703+#501 (G56)
#2704=#2704+#501*10 (G57)
#2705=#2705+#501 (G58)
#2706=#2706+#501 (G59)

M99
%

Any in will be greatly appreciated,
Chris Kirchen

[HuFlungDung]

Limitations of G43? What are you referring to? A G43 length offset is not supposed to show up on the Z axis display in the work coordinate system because the intention of the length offset is to bring the all the tools in a set to a common plane.

I think you need to explain how you are setting up your tools and why you think you cannot trust the machine to handle length offsets. No use creating a handicap style of programming that just makes things difficult for yourself.

[ckirchen]

My intent was not to discuss G43. I am more interested in why changing the G57 work offset with a formula would cause a 0.1 factor to be applied, especially when the same formula works just fine for the other offsets. G43 aside, the problem is still there.

But, while we're on the topic, I guess if I was using G43, I wouldn't have to use a macro, and thus could avoid the problem. I also have a Haas; I use G43 on it all the time and it works extremely well. Basically, I wrote the macro so that the Fanuc would behave like the Haas. When I command G43H02Z0.5 on the Haas, the offset is first applied to the Z DRO (without Z axis movement, work offset table is not changed) and then the tool tip is moved to Z0.5. On the Fanuc, G43H02Z0.5 is treated like G43H02 (Z0.5 is ignored), and if the H is positive, the Z axis runs into the upper limit and faults out.

But it's been almost 6 months since I wrote the macro, so maybe it's time for me to change my programs. I think if I include a line to move Z down if the offset is positive, that might solve my problems. I just need to make sure the I don't do anything for negative offsets. Or is there a way to force the Fanuc to move to Z0.5 like on the Haas?

[HuFlungDung]

I wasn't intending to be insulting or condescending, for the record Just I can't see solving a problem that really need not occur if possible.

I am familiar with controllers that want to execute the length offset (mechanically) as soon as it is encountered. IMO, this limitation can be overcome by the method you use to set length offsets. This has been discussed in several places on these forums. What it boils down to is this:
Set the tool length to a reference block that is higher than your part. The length should be negative, always, for safety sake. No switching back and forth between positive and negative values because sooner or later, you'll have a typo and it won't be in your tool favour.

As you indicated above, call the tool length offset on its own line. This should cause the tool to move to your gage reference plane, and it will be safely above the part.

The difference between your gage and the part Z0 will be a constant, this can be measured and set as a Z value in the current work offset. This amount should remain basically fixed for the duration of your program.

Define your rapid clearance plane as you usually would above the part. The difference between the gage height and the part should still leave the tool at a safe distance above the part when it is at its rapid clearance plane.