Centroid Community CNC Support Forum

How do I do this? I have T1 setup with a different offset than T2 and for example purposes lets say T1 is 2 mm longer than T2. I have Z set at -100 WCS. If I issue T2 changing from T1 to T2, I would have expected the spindle to lower 2mm and the DRO (WCS) to stay the same or the DRO (WCS) to change by 2mm when I issued T2. This did not happen. I can see where this might not happen until the next move so I tried to tell it Z50; then T2; then Z-50 but I ended up at the same place. Not 2mm lower or higher.

I'm not looking for help with settings, offsets etc. but rather is my expectations on what to expect correct.

Thanks Greg

Not an expert but I believe that you also have to call the tool height. T2H2.

I'll see if I an find more on this for you.

MDI

G43H2 ;use tool #2 height value

G43H3 ;use tool #3 height value

greglwood wrote: ↑Fri May 12, 2023 2:02 pm How do I do this? I have T1 setup with a different offset than T2 and for example purposes lets say T1 is 2 mm longer than T2. I have Z set at -100 WCS. If I issue T2 changing from T1 to T2, I would have expected the spindle to lower 2mm and the DRO (WCS) to stay the same or the DRO (WCS) to change by 2mm when I issued T2. This did not happen. I can see where this might not happen until the next move so I tried to tell it Z50; then T2; then Z-50 but I ended up at the same place. Not 2mm lower or higher.

I'm not looking for help with settings, offsets etc. but rather is my expectations on what to expect correct.

Thanks Greg

Your expectations are correct but as CNCMaryland and Keith mentioned you are missing the part to actually activate the tools height offset. When you look at a job file created by a CAM system you will usually see a tool change command T1 M6 followed by the command G43 H1. After the G43 command does activate the tool height offset H1, you will see the change of the DRO Z value if the DRO is in WCS mode and not MCS mode.

Always look at the top center of the CNC12 screen to verify if the tools height offset is active or not. If you see T1 H---, the height offset is not active. If you see T1 H1 you have confirmation that the height offset is active.

Also be aware that CNC12 does allow to assign any H# to any T#, so it could be possible that T1 does have the height offset H2 assigned as an example.

If you are using the ProbeApp (I believe you do), the Tool Library Manager will highlight any H# that does not match the T# to make it easier to spot anomalies (or errors made in the past by playing around with the CNC12 Tool Library).


In the example above, look at 8) where T20 has the height offset H10 and Diameter Offset D10 assigned and are highlighted.

Hope this helps.

-swissi

Thanks to both of you. After playing around with what you both entered I found out the H command is completely independent of the g43 or t command. g43 has to be entered to turn on compensation. After that H1 offsets to the offset in the tool table for 1, but seemingly is completely independent of the tool. It is as if there are 2 tables; an H table, that could be somewhere else unrelated to the tool. H1 changes the offset, H2 changes it, but the tool does not change. g43 can be entered without an accompanying H. G49 turns off the compensation but G43 will turn it back on and it seems to remember the last H regardless of the what it thinks T is.

So it appears that once G43 is on by doing G43 by itself, H# will change the offset and it has nothing to do with the T#. One could enable the compensation with G43 H2 or could just do G43 then later do T2H2 or could do T1H2 and all 3 would set the offset to what is in tool 2.

Maybe this is obvious to everyone else but I have never used offsets before so I guess I assumed the offset had something to do with the tool. I guess it does from a logic and keep it straight in your head kind of way but not from the software's standpoint. From the controllers standpoint there is no connection other than appearing on the same screen side by side. Fusion and other I guess thinks of it as a connection because it has to issue the H# based on the T#.

Can someone tell me of a situation you would want to make the offset different on the same tool. In other words, why would you want do so something like this. G43 T1H1; Position somewhere and cut; T2H2; position somewhere and cut; T1H2; position somewhere and cut. After T1H2 the same cutter that has not changed is now located at a different offset. I'm sure there is a reason but I can't think of one. Why aren't tool and offset joined at the hip?

You can use multiple offsets to control depth of cut without having to write new g-code. For instance, you can do a roughing cut with a face mill at H1, and a finish pass by just changing to H11 which was set 0.005" lower.

Diameter offsets work the same in that they are independent of the tool number.