LinkBack URL
About LinkBacks
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.
| | |
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?
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.
http://www.kirkcon.com/
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?
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. :-/
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.
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.
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.
http://www.kirkcon.com/
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?
you may be misinterpreting the parameter for offset inclusion. you want it set so that the current position does not include the wear offset. the geometry offset must be included in the position readout, but not wear. then your readout will show only the programmed position.
check parameter 3104 bit 6 and bit 7
bit 6 = 0
bit 7 = 1
3104.6 DAL Absolute position
0 : The actual position displayed takes into account tool length offset (M
series) or tool offset (T series).
1 : The programmed position displayed does not take into account tool
length offset (M series) or tool offset (T series).
3104.7 DAC Absolute position
0 : The actual position displayed takes into account cutter compensation
(M series) or tool nose radius compensation (T series).
1 : The programmed position displayed does not take into account cutter
compensation (M series) or tool nose radius compensation (T series).
OK. I looked at this again this morning after a cup of coffee and realized that what I'm seeing seems backwards. I realize it's still my interpretations of things, but the Fanuc parameter guide does a poor job explaining this.
When I started, all four bits (DRL, DRC, DAL, DAC) were set to zero. With the parameters set this way, executing G43 would cause the tool to move to the appropriate offset position AND the DRO value would change. This is what was messing me up initially, because my understanding would be that only one or the other should happen. Either the machine should apply the offset by moving the tool (leaving the position unchanged), or the indicated position of the DRO should be updated to reflect the position including the tool length without actually moving the tool.
In my sleep deprived haze last evening, I changed all four values to 1 just to see what the end result would be, and it appeared to resolve this. Applying a G43 H1 tool length offset now causes to machine to apply the offset by moving the tool to the appropriate offset without changing the value indicated by the DRO.
I'm trying to also understand the reference to wear versus tool geometry as it applies to the readout position. The way the parameters are worded is a little bit confusing because for one value, they talk about the actual position displayed, and for the other they talk about the programmed position. I'm not sure if this is just a fluke in the wording or what. It's almost like saying set the bit to 0 if you don't like apples, set it to 1 if you do like hamburgers.
That aside, what you are saying is that I would normally have it set so that it does include tool length 3104#6, and then doesn't include comp 3104#7?
So, If I'm understanding this correctly I would set it up to include the tool length offset (3104#6=0) and then not include cutter comp (3104#7-1)?
Well, you are still moving the tool. Maybe that is what is throwing you off. My example was to just execute the offset and watch the DRO change with no movement. If you want to execute a move after seeing the DRO change, do that. But look at the numbers on the DRO before the movement and after the movement and I think you will get it.
http://www.kirkcon.com/
Posting Permissions
| | |
