How to setup the Probe for measuring Z with ATC

[erickroyer]

Hi,
I have a machine with an 8 bin rotary ATC. I have a tool setter which I use for measuring tool lengths and I have the centroid probe, which as $699 and I have never used it. I also have a Haimer 3D sensor probe. I understand how to use the Haimer and centroid probes for locating X and Y, but I am really stuck on Z.

Example, If I put the probe in and use Acorn to probe Z it will do that. But... how does the system know the height difference from the tip of the probe to the tools in the ATC rack? How do you measure this.

Using a base tool - Currently I have Tool 1 as my base tool with 0 Height. All my other tools are in relation to that tool. So when I run a job I touch off tool 1 to the material surface and then zet the WCS to 0 and all is good with the rest of the tools. But I want to use the probe (or the Haimer). If I use the probe then tool 1 is no longer the master tool... the probe would be. But how do i tell Acorn the length of the probe (once it touches off) in relation to the rest of the tools in the rack.

I have been looking everywhere for a video or some instructions on this. No luck. I am just worried that if I use the probe for Z and I do not have this setup correctly then when the job starts the Zero reference would not be correct and either crash the machine or not even engage in the material.

Any help on this would be appreciated.

[centroid467]

Hello,

You would use the touch probe as the reference tool for the offset library. Do you have a toolsetting device like a TT-1, TT-4, or surface plate? If so, then you set the Z reference using theKP-3 on the tool touchoff. Next, go through your offset library and get the new height offsets for each tool.

If you do not have a tool touchoff then you'd use the KP-3 to set Z reference on a suitable surface and manually measure the height offset of each tool.

[erickroyer]

My machine has a tool setter like the TT-4 (a different brand). and I have the KP-3 from you. Forgive me, but what do you mean "set the Z reference using the KP-3"? Sorry I am new with this machine and your software. so I would rather ask a lot of question and be sure rather than break something. When you say "get the new height offsets for each tool", do you mean using the tool setter? because that is what I do now.

[centroid467]

Load up the KP-3 into the spindle, plug it in, and use it to touch off on the toolsetter like you would any other tool. You do this to set the Z reference in the tool offset library (F1 Setup > F2 Tool > F1 Offset Lib. > F1 Z Ref). To be more specific: if you have it wired such that the toolsetter and KP-3 can be used at the same time then plug both in. Otherwise, plug in whichever device has the weaker spring.

Yes, after that you should use the toolsetter to get the new height offsets.

Please do not hesitate to ask if you have more questions

[Nigelo]

Eric
From the FB Group in connection with using Z HOME as the reference point from which all tool offsets would be calculated, you asked

How do you set this up with Acorn? you said "change to parameter 3". What is that? Where do you find it? If I understand correctly, you home the machine, put the probe in. When you lower Z and the probe light comes on, then that Z measurement on the DRO is how far down in Z the spindle had to move for the probe to engage. But this number will change depending on the height of the part, no? I am not sure why I find this so confusing... I guess my hang up is that I understand how to set up all the tools using the tool setter, but how does acorn know the difference between the tip of the probe in the baseline for all of the tools?

which I answered as follows:

Parameters are used to setup your machine. Access from the Main Menu using F1 Setup / F3 Config / enter Password (default 137) / F3 Parms. However, it's ESSENTIAL you consult and understand the relevant section 15.3 of Mill Manual before changing any parameter - Manual available from main menu F7 Utility / F6 User Maint / F2 manual.
I think you are confusing setting Machine Coordinates (MCS) with Work Coodinates (WCS). When Remember that when homed , MCS is always zero for all axis. Therefore when setting tool heights using fixed toolholders and Parameter 3 set to use Home, the distance is measured from Z home to your toolsetter for each tool INCLUDING your Probe which is defined as a tool, typically T10. These distances are recorded in the tool offset library and are MCS coords not WCS.

When you come to setting up your workpiece you are then using WCS. If you touch off the Z axis on your workpiece with your probe T10 and save, your job can run with any tool previously saved in the tool offset library - The software calculates the height offset difference between your T10 and the tool actually being used. REMEMBER that its important to set and use the same WCS for your Job and is the reason you will have several WCS to choose from.

See Section 5 of the above Mill Manual

Hope this helps

[cnckeith]

https://centroidcncforum.com/viewtopic.php?f=60&t=6149