[tcom-frazzled]

I just finished installing and setting up a renishaw nc3 on my cnc router. Since the machine doesn't have an ATC, I set it up so that Txx calls macro 9000 for a tool change. In the macro, I have the machine go to a predetermined manual tool change location, wait for the manual change, then on cycle start it executes the tool measurement macro., sets the active tool with a m6 T#149, and returns to the calling program.
The issue I'm having is that after returning to the program, z moves are not going to the commanded height, almost like it is applying the offset twice. I can watch the program zipping by and the commanded z height is not being followed. Oddly, if I jump out with a reset and go to the MDI, commanded Z heights are fine.
Anyone have a thought on what might be going on here? After tool changes, the code calls a g43 h to apply the offset.

[dcoupar]

I'm guessing this must be some super-secret proprietary macro, or you probably would've posted it here so maybe someone could figure out what it's doing.

[txcncman]

Would need to see the code.

[mick.w]

is it possible the probe is resetting your tool #'s, we had a similar problem and we simply recall our tool #'s using goto function

mick

[tcom-frazzled]

Nothing secret about the quick toolchange macro, I'm just not in front of the machine right now to grab the code to post it.

The thing that is really confusing me is that the running program is calling z moves that specify negative coordinates, like z-0.0125, but the position in the current workpiece coordinate system where it ends up is almost an inch higher. If I reset while it is cutting in air and go directly to the MDI, I can issue a g01 z0.125 f20 and it goes to the appropriate position without issuing any other commands.

I've checked the tool offsets and the macro programs them correctly. When it goes back to the program, the correct tool number is indicated, the correct H and D values are specified, and G43 is active. I'll post code this evening.

[txcncman]

Is it stuck in G91 Mode?

[tcom-frazzled]

So, they say a picture is worth a thousand words. Here is a capture of the screen showing the just executed retract G00 Z0.4 that had been executed and look at the Z position on the screen. You can also see from this screen cap what modal G codes are active. Maybe this is just a lack of understanding on my part about how tool length offsets appear while the machine is running, because if you look at the two attached screenshots, you'll see that it is exactly the tool length above the workpiece while running.

[txcncman]

What is in the G54 offset for Z?

[tcom-frazzled]

Z offset is -4.2390. I used the tool change macro to install tool 1, then used the MDI to execute a G43 H1 to set the offset active. After which I touched off the top surface of the material and used the indicated Z position to input the offset.

Maybe it is just my understanding of how G43 works that is the problem. When jumping between G49 and G43H1, I would expect the Z position to remain the same on the DRO and just the tool length offset to be applied and to tool to move in the positive direction by the distance of the length value. What I'm seeing is that when I jump between G49 and G43 modes, the DRO value changes.

[txcncman]

Oh. No. I think I am understanding now. What I am not seeing is if you confirmed the DRO tool position is the actual tool position in the machine. If the DRO is reading 1.4126 positive above the set Z work zero, is that the actual distance from tool tip to the set Z work zero in the machine?

[tcom-frazzled]

Yep, that is the actual position of the tool above the workpiece when this is running.

[txcncman]

Ok. Then yeah. You were misunderstanding the order of operations for the DRO to get where it is. Sorry for the misunderstanding and bad communication. If the DRO says the tool tip is at 1.4126" above the Z work zero and it physically is that distance, then all is well.

[tcom-frazzled]

RIght. What I'm finding confusing is that the program is commanding a move to Z0.400, but it actually moves to Z1.4126 instead. I guess I'm used to the offsets being transparent and that after applying a tool length offset, when I commanded something to z0.400, that would be the tool tip coordinate at the end of the move. Since offsets weren't being used on this machine before, maybe I'm missing something with parameters that need to be set to control this behavior?

[txcncman]

Offset in the table should be negative value for G43. I think you can use positive values with G44. Sorry it has taken so long to catch that.

[tcom-frazzled]

Hmm. Admittedly I'm coming from running a machine with Mach 3 for a long time so there are definitely a few differences. My understanding of the tool length offsets are that a location (typically the spindle nose) is selected as an offset reference location. When G43 H1 is called, the length of the value is added to the spindle position, thus moving it up by the length of the tool so that the new zero point is at the tool tip.

What I'm not getting is that if I switch between no tool length comp G43H0 or G49, and tool length comp G43H1, the DRO value changes along with the tool move. In G49, shouldn't the tool length offset be cancelled and the displayed Z coordinate be referenced to the spindle nose (or whatever spindle zero reference is being used) instead of the tool tip?

[tcom-frazzled]

Looking at the parameter manual, it appears I need to go through the 5001-5040 parameters and double check them as well. Some of this oddity could be coming from things like 5001#6 (EVO) which defers G43 offset application until the next G43 call. Gonna double check that now, as things like that would make the G43 offsets behave in really strange ways. :-/

[tcom-frazzled]

Let me ask a simple question that should help me clarify this. If I single step through the following lines, assuming the length offset value for tool 1 is +1.0000, I'm using inch units, the current position is Z1.000, I'm in absolute coordinates, and I'm starting with modal G49 active:

G43 H1 G00 Z1.000;
G49 G00 Z1.000

When activating G43, I would expect the machine to move Z+ by one inch, but the DRO to read 1.000. Upon executing the G49, I would expect the machine to move Z- by one inch to cancel the offset, but the DRO to continue to read 1.000.

The behavior that I see is that the offset is allied or removed as appropriate, but the DRO value also follows the tool tip? If that is expected, so I not need to use G43 tool length offsets because the machine already applies them somehow when the tool number is called?

This is on a 21i-MA if that matters.

[tcom-frazzled]

OK, some more digging and I now think I understand what is going on. Some additional digging around the internet brought up discussion that the display can be set to either include or not include the active offset based on a parameter setting. Given the way this machine is behaving, it apparently isn't set up for the display to include the active offset. This is gong to make me insane over time, so I need to figure out the proper parameter to change it for the 21i and set it so that the DROs include the currently active offset.

[txcncman]

Let me see if I can walk you through this. First, start with a clean slate. Power up the machine and home it. Look at both machine position and absolute position on the DRO for Z. For most machines, both should read 0.0000 right now. Now, in MDI, execute G43 H1 with no work zero shift. Since you used positive numbers in your tool offsets, the DRO should read 1.0126 for Z absolute. Machine position should not have changed. Now execute G49 and should take you back to 0.0000 for Z on absolute. Now execute G44 H1 and DRO should read -1.0126 for Z for absolute. I hope this helps you sort things out in your head.

[tcom-frazzled]

I got it figured out. What you say is true and how the machine was behaving, but it isn't what I'm used to. I'm used to the DRO showing values that reflect the state of tool length offsets. Where this was messing me up wasn't with the tool offsets, but rather with the workpiece coordinate Z offset. Because the tool offset wasn't reflected in the values shown on the position screen, I was setting up the Z height of the workpiece using values that didn't include it. This meant that whenever I would go to cut, all of my z depths would be higher than what I wanted by the amount of the tool length.

For me, the easier solution is to have the DROs show the position including any tool length offset so that the tool tip is always referenced when G43 is active. Some reading of the parameter manual led me to parameter 3104,#4-#7 (DRL, DRC, DAL, DAC). These parameters on the 21i determine whether the DROs for relative coordinates (DR values) or absolute coordinates (DA values) include the tool length offset or not. On my machine they were set to 0, which does not adjust them for tool length compensation when active. While I'm sure arguments could be made both ways on how these should be set, my life will be a lot easier if the displayed positions reflect active compensation, so I have set these to 1 and now the readouts behave as I am used to.

Just so I can understand the other side of this setting, why would you not want the DRO to reflect compensation when it is active? Is there a reason why someone would want the DRO to always reference the spindle nose's relationship to the workpiece as opposed to the tip of the active tool?