Tool change and loss of WC Z0

[yeeter]

Not a crisis since I moved on to a tool library, but I make a lot of tool changes so may want to come back to this at some point:

When a tool change is made the WC Z0 resets to that tool, losing the original working zero.

As mentioned it is not happening with the tool library option. Only the option that touches off after each new holder is picked up.

Am sure this is something simple... any thoughts on approach to resolve? ( I can post all the macros if needed, but was guessing this is something basic - such as the ATC initialize or such )

[yeeter]

And just an example - once the z height resets I then get the error that z height is exceeded.

If I manually reset WC Z0 and it does not require a tool change, then it runs as expected. So it only happens due to checking the tool height after a tool change.

The mfunc6 macro is stock as exported via the Wizard.

I tried putting a value into Parameter 70 seems no effect.

[Ken Rychlik]

Top of your screen.... T2 H--- is never going to give good tool offsets. If you don't have T2 H2 on top, you have not gotten things set up. Your toolpath is doing a G43 calling for the tool offset, but there is no tool H# for it to even pick from.

If you don't want to track tool offsets, your design program should not be asking for the G43 tool offset.

It also looks like you have some Z soft limits set. I don't normally use those, but those settings could also bring more challenges.

One more thing I noticed on your toolpath. M3 S10000 is ok buy why is there a feed speed on that same line? For what you are trying to do, you might need to modify your post processor in the design program.

If you post a fresh report, someone can probably pick out what's going on.

[yeeter]

Yes. But with option 1 for the ATC (measuring tool length after every swap), there is no T1 H.. That I can tell. (in tool library setting option 2 there is).

The design program is Vectric Vcarve Pro and the canned centroid post processor it finds on the cloud. Tool library is defined the the Vcarve toolpath definition (the only way to get two separate toolpaths in Vectric, is to assign tool numbers). The resulting file calls for the swap so part of it is behaving.

I 'thought' I had it with a negative offset value in Parameter 71 - but again that was over written on the next tool swap.

It is the tool touchoff that is resetting Z.

Reading about coordinate 'modes' .... some references here on G90/91/other coordinate modes not being in the right place at the right time. At one time I did make M6 edits to add some clearance moves so those may have caused the coordinate mode to switch on me.

I am stll learning basics - not sure what Mode the WCS is. (not G90/91 perhaps something else)

[yeeter]

All telling report attached

[yeeter]

As far as how I would 'like' to use it (reset me from scratch, I think this is designed for it but I am off track somehow) :

The purpose is to be able to swap out tools for a particular job. No permanent assignment per se (although I bet 3 of the 5 remain the same always, and a couple of them get swapped depending on task at hand).

Then secondly I would like the choice of zeroing on the spoil board, or zeroing on the top surface of the workpiece. Again depending on task at hand.

I do have a permanent spot with a tool touchoff mounted.

Then ideally can use a second material touchoff to set the zero reference for that particular job. (currently this is not wired, simply referencing manually using a tool at the moment - it specifies which tool is used)

So the material reference should be made. Then each tool would go to the fixed TT location and measure from absolute machine reference and make the corresponding translation for the tip of that tool to the material reference (but as noted right now the TT resets Z - not to the material).

What is the proper way to configure this? (the Wizard does not treat me well, I prefer to understand what it is doing)

Some specific questions:

What should parameter 3 be? (one of the guides suggests para 4 be set to 6 but that looks incorrect although a fairly current guide - appears to be parameter 3)
Where should the TT offset be loaded? Parameter 71? Negative or Positive? At all?
Is the TT offset measured from spoil board? Or how far down in Z ref until tripped? (assuming this is parameter 71) Or again perhaps not necessary.
Does the material offset in setup, and the WCS Z0 do the same things?
If the tool is being measured each time, what is the purpose of the tool offsets? (just a starting point?)

[cnckeith]

hello.
i'd suggest you use the latest version of CNC12 software now available which has improvements and additions in this regard in both cnc12 and the setup wizard.
more information can be found here.
https://www.centroidcnc.com/centroid_di ... loads.html

your license file will work with it and its free.

also your existing v5.1 install will completely be retained and intack and you switch back to it if you like at any time in just seconds.

[CC810]

I had this same issue with the stock M6 program for the ATC.
Using a fixed tool touch off and Z home = Z ref
I ended up using the tool offset library and replacing on line 210 "G92 Z[0-[#106]]" -- this basically resets the WCS Z0 at this point
and replacing with "G10 H[#12000] R[#5023]" -- this writes the Z value from Z home to the tool H value in the tool library

So every tool change the tool is measured at the fixed TTO and WCS is not reset
This way i can put all the tools required in the forks and it just measures at every tool change. Once the WCS Z0 is set at the spoilboard or stock top its not re set and every tool change is compensated for.

One other thing i added some skips in the macro to skip the tool load and skip the TTO sequence if tool zero is entered. This way it allows to unload the tool and not load the next one. the loaded tool T is set to zero and the tool H is set to zero. So then i added M6T0 to the park.mac so at the end of the machine use it will unload the tool to T0 and then park with the spindle unloaded

[cnckeith]

I had this same issue with the stock M6 program for the ATC.
Using a fixed tool touch off and Z home = Z ref
I ended up using the tool offset library and replacing on line 210 "G92 Z[0-[#106]]" -- this basically resets the WCS Z0 at this point
and replacing with "G10 H[#12000] R[#5023]" -- this writes the Z value from Z home to the tool H value in the tool library

So every tool change the tool is measured at the fixed TTO and WCS is not reset
This way i can put all the tools required in the forks and it just measures at every tool change. Once the WCS Z0 is set at the spoilboard or stock top its not re set and every tool change is compensated for.

One other thing i added some skips in the macro to skip the tool load and skip the TTO sequence if tool zero is entered. This way it allows to unload the tool and not load the next one. the loaded tool T is set to zero and the tool H is set to zero. So then i added M6T0 to the park.mac so at the end of the machine use it will unload the tool to T0 and then park with the spindle unloaded

cool. that's why all the macros are editable so you can tweak it the way you want!

post a fresh report.zip so we all can see what you did.