Build Thread Mach3 to Acorn

[cnckeith]

looks like you really should be using a Touch Plate not a TT for your work flow if you are just always resetting part Z zero with each tool. an TT is not necessary for this work flow.

TT = used for measuring tool heights

Touch Plate used for setting WCS (part zero positions)

[Leo Voisine]

I am aware that the TT is for measuring tool heights. Measuring the tool heights seems to be working as expected. The numbers in the tool height registers look reasonable.

What seems to be happening is that part zero seems like it is changing every time I measure a tool.


I bought Centroid and the TT4 for this reason - to be able to change a tool, remeasure and continue
The video from Clint https://centroidcncforum.com/viewtopic.php?p=9150#p9150 seems to do exactly what I want to do.

In Mach3 - I would touch each tool to part zero and I am sure that will also work in cnc12, but I want something better, hence acorn. Doing the tool change the Centroid is just soo much better - IF - I can get it to work.

As advertised at $660 for the TT4 probe, I would hate to say - oh well - I don't need that anyway. OUCH

There must be a way

[ShawnM]

Again, the M6 macros in that topic posted by Scott (sword) assume you have a movable tool touch off. The is for the initial setting of Z0. That is either the work surface or the spoilboard surface, doesn't matter. Your fixed tool touch off only comes into play once you have set part zero with the first tool with the movable tool touch off. You have to load your first tool and touch off and set part zero, then and only then will the M6 macro move the tool to your FIXED tool touch off and record an offset. It does not record or set the length of the tool in the collet. And there's no need to know the height of your fixed tool touch off. And you do not enter its height in the wizard for the height of your tool touch off. The height you set is for your movable tool touch off.

Once you set part zero, with a movable tool touch off, your fixed tool touch ONLY measures an offset value. It does not measure the "tool length" or store a "tool length" anywhere. It simply records and stores an "offset" value to use during the next tool change.

You should not be doing anything in the ATC menu as you do not have an ATC. All that is going to do is confuse you even more.

You need to modify the posted M6 macros to do the following: (if you don't plan on adding a movable touch plate of some sort)

after you load the job and press cycle start it should:
prompt you to manually insert tool one in the spindle, press cycle start to continue
prompt you to manually jog the machine to set part zero, press cycle start to continue

at this point the macro should then move to your fixed tool touch off and touch off and record the offset then start cutting.

When it comes time to change to the next tool in your program your M6 should then turn off the spindle and move it to a predefined "tool change location".

You should then be prompted to change to tool XX and press cycle start to continue.

This is where you change tools and press cycle start. When you change the tool and press cycle start it will then move back to your fixed tool touch off and measure this new tools offset and add or subtract the difference from the last tool and then start cutting the next tool path.

This will repeat for as many tools in yout job g code.

There is nothing for you to set in the ATC menu and no tool to auto measure. In fact there's no reason for you to ever go in the4 ATC menu.

But none of this will happen with the M6 macros found in the topic I linked to because they all assume you have a MOVABLE tool touch off along with your fixed tool touch off.

You need a custom macro if you are not going to add a movable touch plate to your setup.

[Sword]

Agreed. If it would help, I can make a video of the exact sequence as Shawn stated (without a touch plate), but not until sometime later tomorrow.

[Leo Voisine]

Again, the M6 macros in that topic posted by Scott (sword) assume you have a movable tool touch off. The is for the initial setting of Z0. That is either the work surface or the spoilboard surface, doesn't matter. Your fixed tool touch off only comes into play once you have set part zero with the first tool with the movable tool touch off. You have to load your first tool and touch off and set part zero, then and only then will the M6 macro move the tool to your FIXED tool touch off and record an offset. It does not record or set the length of the tool in the collet. And there's no need to know the height of your fixed tool touch off. And you do not enter its height in the wizard for the height of your tool touch off. The height you set is for your movable tool touch off.

Wonderfully said. I set the part zero surface directly with tool tip to work surfece as I do not mave a movable TT. End result is exactly the same. Movable TT is just easier.

Once you set part zero, with a movable tool touch off, your fixed tool touch ONLY measures an offset value. It does not measure the "tool length" or store a "tool length" anywhere. It simply records and stores an "offset" value to use during the next tool change.

OK - so this may be the issue but I don't know how to resolve it. This may be what the method 1, method 2, or method 3 is about and this may be where my problem is. I am pretty sure it is in the method of how the wizard is set up. At this point I understand that I should NOT use the slider to subtract the TT4 height. That slider is set to NO

You should not be doing anything in the ATC menu as you do not have an ATC. All that is going to do is confuse you even more.

I tested the Auto Measure in the ATC menu vs MDI T# m6 -- both give same result. I can just use MDI and M6
Other thing is the tool library is there.
I can ignore the ATM menu as long as I get good results in the machine
I am not really confused just a little frustrated
I have 40 years working with industrial machines

You need to modify the posted M6 macros to do the following: (if you don't plan on adding a movable touch plate of some sort)

after you load the job and press cycle start it should:
prompt you to manually insert tool one in the spindle, press cycle start to continue
prompt you to manually jog the machine to set part zero, press cycle start to continue
This is where I do the part zero manually

at this point the macro should then move to your fixed tool touch off and touch off and record the offset then start cutting.

When it comes time to change to the next tool in your program your M6 should then turn off the spindle and move it to a predefined "tool change location".

You should then be prompted to change to tool XX and press cycle start to continue.

This is where you change tools and press cycle start. When you change the tool and press cycle start it will then move back to your fixed tool touch off and measure this new tools offset and add or subtract the difference from the last tool and then start cutting the next tool path.

This will repeat for as many tools in yout job g code.

Everything between my last comment and this comment is completed and is working flawlessly. the only exception is the movable plate to set part zero. That should be a moot point


There is nothing for you to set in the ATC menu and no tool to auto measure. In fact there's no reason for you to ever go in the4 ATC menu. OK, I am good with this

But none of this will happen with the M6 macros found in the topic I linked to because they all assume you have a MOVABLE tool touch off along with your fixed tool touch off.

I am a bit familiar with macro programming. I added an unconditional loop to skip over the movable plate as I do it manually You can see that in my Mfunc6.MAC When I get set up with a movable plate I will set that up in the M6 macro.

You need a custom macro if you are not going to add a movable touch plate to your setup.
I have that

Guys - I 100% agree with you. My work sequence is exactly what you are saying. I am doing exactly what you are saying.

Only one difference. Setting part zero on a movable plate and setting part zero.
I set part zero from tool tip directly on part zero surface instead of using a movable touch plate. There is NO difference. If there is a difference - what is that difference?

Avid CNC is doing EXACTLY what I want to to
In the video he does use a movable touch plate in one example BUT he ALSO does it the way I do it in another location



I know this is possible - it's all in HOW it's set up.

This work process is a game changer, Centroid Rocks in this ability

[Leo Voisine]

Agreed. If it would help, I can make a video of the exact sequence as Shawn stated (without a touch plate), but not until sometime later tomorrow.

I am sure that will help - I can do the same.

I would also be very appreciative of youe effort in that endeavor.

[ShawnM]

I tested the Auto Measure in the ATC menu vs MDI T# m6 -- both give same result. I can just use MDI and M6
Other thing is the tool library is there.
I can ignore the ATM menu as long as I get good results in the machine
I am not really confused just a little frustrated
I have 40 years working with industrial machines

The auto measure has nothing to do with this M6 macro. Once again you should not be setting anything in the ATC menu or the tool offset library. This M6 macro assumes there's no ATC or offset value setup for any tool. If you set any values in the offset library it'll mess up this macro for sure.

The Avid video you posted is not the same procedure as the M6 macro found here. That's not how this one works. It does however use a movable tool touch off which again is the conventional way that people use the M6 macro you found here.

It can be done but you'll have to setup the wizard differently than the macro directions say to and you'll have to make some menu changes in the macro and change the way the initial Z zero is set since you dont want a movable tool touch off.

[Leo Voisine]

I tested the Auto Measure in the ATC menu vs MDI T# m6 -- both give same result. I can just use MDI and M6
Other thing is the tool library is there.
I can ignore the ATM menu as long as I get good results in the machine
I am not really confused just a little frustrated
I have 40 years working with industrial machines

The auto measure has nothing to do with this M6 macro. Once again you should not be setting anything in the ATC menu or the tool offset library. This M6 macro assumes there's no ATC or offset value setup for any tool. If you set any values in the offset library it'll mess up this macro for sure.

I promise I will never again touch the Tool/ATC menu


The Avid video you posted is not the same procedure as the M6 macro found here. That's not how this one works. It does however use a movable tool touch off which again is the conventional way that people use the M6 macro you found here.
It does BOTH - he also manually sets part zero

It can be done but you'll have to setup the wizard differently than the macro directions say to and you'll have to make some menu changes in the macro and change the way the initial Z zero is set since you don't want a movable tool touch off.

Awesome news - It can be done
How do I - set up the wizard differently
How do I - change the way the initial Z zero is set
How do I - make some menu changes in the macro

Thank you for responding

[ShawnM]

I promise I will never again touch the Tool/ATC menu

LOL, good to know.

Since you say you have macro experience, in that topic I shared where Scott posted the various options for tool setting you will want to combine two of them to make it work.

Option 1 is manually setting Z zero without a movable tool touch off. Start here, combine the first half of this macro with the second half of option 4, the one labeled mfunc6_clint.mac

This will get you what you need.

As for your wizard settings for tool touch off for this custom macro,

-tool measurement ref method should be "z home=z ref"
-use touch probe as ref tool should be "no"
-subtract height of tool touch off device should be "no"
-use fixed tool touch off (TT) location should be "yes"
-tool touch off/surface plate height should be set to zero

Hopefully this will get you started down the correct path.

[ShawnM]

One more thing, these macros have you setup G28 as your "tool change location" so you'll wan to set those coordinates up also. This is where it'll move to for you to have easy access to change the tool before it moves to the fixed tool touch off location.

Returns are setup here: F1, F9 then F6.

G28 or return 1 is the tool change location you choose and G30P3 or return 3 should be set already because you set the location in the wizard already.

Lastly, these macros were written for older versions of CNC12 so system variables and other things might have also changed.