tool offsets kicking my butt !

How does one simply, by hand, manually add tool lengths ( tool plus holder ) to the tool table and have it compensate with the Z axis when the Z zero is set with a designated tool ( for example a Haimer 3d centering device in a tool holder ).

If the Haimer is say, 6.5 inches, where does this "offset" get input properly. So far, I'm not having any luck with (Linuxcnc 2.7) with regard to tool offsets. What the heck am I missing !?!!?!

My only excuse is, I'm a noob that only has experience with Mach 3, arrrgh, my butt is getting kicked by this, and it should be simple !

Jake

If your Z0 is a tool length of 6.5" the tool offset should be equal to however much longer or shorter your tool is. So if T1 is 7" the T1 offset should be +0.5, if it is 6" then it would be -0.5.
You can enter this number either by directly entering the tool table, or after the tool is loaded using the tool touch button (in the Axis UI.) or using a G10L1 command linuxcnc.org/docs/html/gcode/g-code.html#gcode:g10-l1

Don't forget you have to enable the tool length offsets by issuing a G43 (Hn) command in the g-code after the tool is loaded for the offset to take effect.

Todd Zuercher wrote: If your Z0 is a tool length of 6.5" the tool offset should be equal to however much longer or shorter your tool is. So if T1 is 7" the T1 offset should be +0.5, if it is 6" then it would be -0.5.
You can enter this number either by directly entering the tool table, or after the tool is loaded using the tool touch button (in the Axis UI.) or using a G10L1 command linuxcnc.org/docs/html/gcode/g-code.html#gcode:g10-l1

Don't forget you have to enable the tool length offsets by issuing a G43 (Hn) command in the g-code after the tool is loaded for the offset to take effect.

I guess I assumed that "in this day in age" we wouldn't have to pull out a calculator at all since this should be done by the "confuser aka : expensive calculator " by designating a "manual" probe height / tool zero , for example: the Haimer at 6.5 inches. The tool table would have been populated with measurements from the base of each tool to the tip of the tool and the table would be updated "automagically" with an offset value to reflect the difference in height ( the same as the value you said I should calculate on my own for each tool ).

Anyway, thanks Todd for that workaround. I'll just use that for now. Much appreciated.

Jake

It is possible to configure linuxcnc to do automatic tool measuring. But you have to know how to configure the machine to do it.

Are you saying your machine has a probe or something like that you can touch off the tool with?

If all of your tools are calibrated for gauge hieght, and your Haimer probe has a gauge height of 6.5" all you would need to do is touch off your machine coordinate system to Z6.5 when you probe (not Z0). Then the tool length for your 7" long tool would be 7" in your tool table.

Todd Zuercher wrote: It is possible to configure linuxcnc to do automatic tool measuring. But you have to know how to configure the machine to do it.

Are you saying your machine has a probe or something like that you can touch off the tool with?

If all of your tools are calibrated for gauge hieght, and your Haimer probe has a gauge height of 6.5" all you would need to do is touch off your machine coordinate system to Z6.5 when you probe (not Z0). Then the tool length for your 7" long tool would be 7" in your tool table.

I suppose I shouldn't have used the word "probe" at all. The Haimer is a "manual" gauge tool.

I believe I tried the same method you mentioned just above but nearly had a crash with a drill bit. Thankfully I was on the ready at the E-stop before it did damage to my vise. Its possible, in my research this morning, I found that maybe I need to issue the G92.1 command to clear up some monkey business that I did trying out the Tool Touch off "command". It seems there is a hidden setting that might need resetting to zero. Not sure yet.... I have not used the G43 command either but used a GUI button to save, and reload the tool table, that I assumed would do the same as G43. The tool table also doesn't stay persistent after the computer is turned off. I come back to the machine after not having turned the computer on for a few days and the tool table is back to its default empty status.

Jake

I'm a little confused about what exactly you have, want, and are trying to do, so I'm not sure what to recommend now.

Important things to remember when using tool offsets.
When making manual edits of the tool table using the tool table editor, you must save it and reload it for changes to take effect. The tool table is saved to a file in your config directory and is persistent and should remain unchanged from session to session. Tool offsets are not applied unless a tool is loaded (Tn M6), and G43 (tool lengths) or G41/G42 (diameter offsets) are active. Try not to confuse machine coordinate offsets G54-G59.1 and G92 and their touch off commands and the tool offset touch off.

Todd Zuercher wrote: I
......
If all of your tools are calibrated for gauge hieght, and your Haimer probe has a gauge height of 6.5" all you would need to do is touch off your machine coordinate system to Z6.5 when you probe (not Z0). Then the tool length for your 7" long tool would be 7" in your tool table.

Hey Todd, The above worked perfectly after I cleared g92.1 and g43 after setting the tool heights.

So that is working now thanks to your help !

The separate problem of the tool table resetting itself to original defaults may still be a problem. Time will tell...
Thanks again,
Cheers,
Jake

The tool table not keeping info on restart of Linuxcnc happened to me also when i did a retrofit of a mill with 8 tool turret.
Had to make the tool.tbl read only to keep the info unchanged.
Did not have time to investigate further as the machine had to go to production.

Just to add another way.

Probe to the top of your table, or the top of a workpiece with the Haimer. This is now your reference tool.
Set Z, in the coordinate system, to zero.

Now put in a tool and jog it close to the reference table. place a dowel of known diameter next to the tool and jog up until the dowel slips under (jogging up avoids the risk of jogging down onto the dowel).
Now use the "touch off tool" button and enter the dowel thickness as the Z offset.
With Touchy you will now need to MDI a G43. I think Axis does this automatically.
You should now find that that tool shows zero when at the reference surface, and the tool table will contain the difference between the Haimer length and the tool length.

Another way is to measure the length of the Haimer in a fixture, and put that in as the probe-tool length (I use T99 for my probe) and then measure the other tools in the same fixture. I built a fixture into the end of my milling machine: . It is possible to enter the values in the MDI window, rather than with a text editor, with Touchy I press the "tool touch off" button then manually change from L2 to L20 (I think, it's been a while)

You can combine both methods, as long as the Haimer is loaded as a tool and G43 is in effect at the time that you probe the reference surface.