Sporter

As I have stated I am new to the use of the Fanuc16m using G43.1 and have not used G43.4 at all. But I do know that if you put a Z command on the block that has the G49 it will go to that location without the gage length when it is executed. So what I did when I turned off G43.1 with G49 (because G43.1 needs to be off for the tool change) was to send the machine to a position close to its max Z (for safety) with the following block G0G49Z30. That way the tool went up and not down when it turned off G43.1 tool length compsation. Maybe that will work with G43.4

I've always finished a G41.1 toolpath with

G91 G28 Z0.

G91 G28 X0. Y0. B0. C0.

G90 G49 G40 G80

M30

Which sends the machine home, then cancels things without any Z move. But this alarmed out on the G91 G28 Z0 line when using G43.4.

So I moved the G49 up

G49

G91 G28 Z0.

G91 G28 X0. Y0. B0. C0.

G90 G40 G80

M30

It works OK, but the tool comes down in Z by the tool offset value on the G49 line.

Parameter 5006 #6 set to 1 stopped this on the newer machine with a Fanuc 18 control. But it doesn’t do the trick on the older Machine with Fanuc 16 control that we upgraded. Our machine supplier is looking into it for us.

I could try adding a Z value to it, but we'd run the risk of over travel/or not enough travel. I'd rather it just went to Z home. I'll mess more if we don't get the parameters sorted.

I’ve never heard of G149?  I’ll give it a try.

SPORTER

I recently had the exact problem that you are talking about, getting the alarm. And I too moved the G49 up as you did. I also had the same problem that as soon as I did, the machines moves to the Z location  stored in memory but without the tool lenght offset so it moves down the value of the stored gage length register. I don't like just putting in a Z30 either (the shop here edits the Z30 value if it overtravels, only because they do not know of any other solution) for the same reasons you mentioned. I will be glad if you machine supplier can come up with a better solution.

On another note, I am also going to ask the Fanuc rep here if there is a parameter bit in the controller that needs to be toggled to calculate the correct inverse time feedrate. I don't think it can be done in the post because the post does not have all the information to accurately calculate time since it doesn't have the gage length of the tool to put into the calculation.