Tool Table Touch Off

I don't think so. The fixture is to measure the relative length of the tool as it would extend from the spindle nose. So if the table has all the lengths recorded from the same fixture then the relative length is all that matters.

If:
T1 is 1.500" long
T2 is 2.000" long

And Lets say I touch off to the material with T1. Now the machine knows that when I switch to T2 the tip is 0.500" closer to the work and can adjust the coordinates to compensate. Assuming that the offset has been loaded with G43.


The important part is that every tool in the table is measured from the same fixture with the same contact point. So for me with R8 TTS tools I measure on a granite plate from a steel fixture that contacts the TTS ring. For a tapered tool the fixture would need to have a matching taper so that every tool fits the taper the same. My mill table position is completely irrelevant to the process. hope that makes some manor of sense.

On our VMC we have a dedicated tool (really just a tool holder with a blank in it) that we jog down to a touch off gauge. This is used to set G54 for material thickness. Then as new tools are loaded they are jogged down to the same gauge and touched off to the tool table. In our case the gauge is a dial indicator that zeros at 2" above the material, but in the past we used feeler gauges, paper, etc. The important thing is to have a tool defined that all the other tools are offset relative to. This is why we don't use that tool!
My pet peeve with the touch off procedure is that it's possible to add offsets other than Z to tools if you are not paying attention. I'll have to look into trying to change that behavior, rather than training the humans to watch out.
Hahn Rossman
www.alkifoundry.com

Sorry to bump an old thread, but this one keeps popping up and is pretty much covers the same question I have...I just seem to be missing a key step or something.

I'm trying to set up my tool table on my mill that uses QC30 holders. I just can't seem to get the results I expect when I try to set up each tool's offsets.

Here's the steps I tried today:

-Set tool 1 with T1 M6 in mdi.
-Faced off piece with T1. Touched off faced part as 0
-Also used "touch off tool" and set to 0. Z showed 0 as expected

-Changed tool 2 with T2 M6 in mdi
-Used 2" touch-off gauge on previous face, used "touch-off tool" and set Z to 2"
-Display showed Z changed to 2" as expected

When I tried changing back to T1, I would have expected it to change the Z offset back so when I touched tool 1 on the gauge, it would read 2" but it was some other random number.


A also notice that changing between tools doesn't seem to affect the displayed Z even though the tools have different Z offsets in the tool table.



Is there any good reference that explains step by step on how to set up and touch off? I have a feeling I'm missing something painfully obvious here, but it's just not coming together for some reason...

You need to also call the offset from the tool table when you change the tool.
Something like :
t1 M6 G43

If you read up about g43 it's got a lot of specifics depending on how you are changing tools.
Depending on you post processor/CAM software you may or may not see this in posted code, but you need it to get the tool offsets to play nice in MDI mode.
Hahn Rossman
www.alkifoundry.com
www.rossmancycles.com

OK, so G43 was definitely the missing link in my mdi tool changes. After adding that and touching off each tool, I saw exactly what I expected in the tool table and changing tools gave me repeated accurate touch-offs on the fixture.

I'm using Fusion 360 with the EMC post. I believe this is the most current one for LinuxCNC.

Looking at a sample of a file I just posted, here's the part containing the 2nd tool change:

I notice it's only calling "T2 M6" with no G43. I just tried running this through this tool change (without tools installed) and it appeared to be holding the correct offsets. I'll be trying to full program with tools next....with my hand held firmly on the e-stop!

I guess I need to do a little more reading on the Fusion post and see how hard it is make it add G43 to the tool changes. I suppose I can add it manually after I post for now, but I know that's just asking for trouble as I'll inevitably miss one and that probably won't end well.


Edit: Actually, looking at it more closely, I see there is a G43 in there on line 155, as it's running the first Z depth. Perfect. It was just my lack of understanding how to set up the tool table all along!

The G43 command is 6 lines below the tool change command in your example. Also, T3 is preset to load on the next m6.

the Fusion 360 CAM has been working well for me for over two years.

Ray