tool z and x ref and offsets discussion for lathe auto tool touch off

[greenail]

In this post I want to attempt to disambiguate the tool references and the tool offsets when using the automated probing and tool setting functions..

The below is a work in progress and is being drafted based on feedback in this thread.

terms:


master tool/reference tool This tool is the reference tool. the best practice is to setup offsets relative to this tool.
slave tool: Slave tools are offset from the master tool in the Z and or X dimensions.

Z ref: the reference position is a temporary position used to measure the difference in length between tools. when adding new tools or updating tool offsets the reference needs to be reset after a re-home or power down. The Z ref does not need to be changed to use the work offsets for jobs after homing or power down.

X diam/X ref: the X ref behaves the same as the Z ref described above.

tool offsets: are the difference in length between the slave tools and the master tool. the tool offset is relative only to the master tool. the z ref and x ref positions have no effect on the saved tool offsets and are only used to calculate an offset measurement when measuring a tool.

Process 1: Establish reference position. This process is used for initial setup and when adding or adjusting tool offsets after the initial setup.

note: If the reference position is established it can be used until the machine has been re-homed or powered down. When setting up multiple tool at one time the reference position does not have to be reset.

1.) home machine
2.) set part X zero with Tool #1 (x offset = 0 Z offset =0) make a skim cut on scrap material, measure diameter, enter diameter in X part zero setup screen press f10 to save.
3.) Insert probe into spindle
4.) Set up X reference position: highlight Tool #1 X offset (0) and press F1 X diam and choose direction, cycle start to seek probe and set x ref.
5.) Set up Z reference position: highlight Tool #1 Z offset (0) cycle start to seek probe and set x ref.

Process 2: setup master tool. This process is used to set or reset the master tool.

1. Establish reference position (described above)
2. highlight the master tool in the tool offset screen.
3. ensure X and Z offsets are Zero. ensure tool wear settings are also zeroed out.
4. save settings.

Process 3: Setup new master and slave tools

1. Establish reference position (described above)
2. setup master tool (described above)
3.) Tool check and Change Tool to the slave tool for setup, jog the tool close to probe. We will use tool #2 for this example.
4.) Highlight tool #2 in the tool library.
5.) Measure Tool X offset: Click measure tool, click Measure offset X, choose direction to move to seek probe, cycle start to seek probe, X offset is now entered automatically after successful probing cycle
6.) Measure Tool #2 Z offset: Click measure tool, click Measure offset Z, cycle start to seek probe, Z offset is now entered automatically after successful probing cycle.

Process 4: Adjust existing tool offset or add new slave tool

1. Establish reference position (as described above)
2.) Tool check and Change Tool to the slave tool for setup, jog the tool close to probe. We will use tool #2 for this example.
3.) Highlight tool #2 in the tool library.
4.) Measure Tool X offset: Click measure tool, click Measure offset X, choose direction to move to seek probe, cycle start to seek probe, X offset is now entered automatically after successful probing cycle
5.) Measure Tool #2 Z offset: Click measure tool, click Measure offset Z, cycle start to seek probe, Z offset is now entered automatically after successful probing cycle.


Process 5: sanity check

to change to tool 3 run in mdi. this says use tool 3 and offset 3.

Code: Select all

t0303

then to jog the tool close so you can eyeball the position. this assumes part Z 0 is setup correctly.

Code: Select all

g0 z5 x0

Questions:

the manual says x diam is "set for OD". it would seem that you should do all your OD tools, reset "x diam" with the reverse X probe seek direction, and then do your ID tools with the new "x diam" from the X+ direction. ?

why do you need to make a cut for x diam and also another for x offset? This seems redundant? Also this doesn't seem to apply to auto tool setting, should the setting instructions for both x diam and x offset be ignored and just set them to 0 to simplify the setup?

how do you auto set the Z offset for something like a neutral 55 degree tool or a threading tool?

why not use "measure Z and X"?

can we make a auto tool touch off establish reference position macro to automate steps 1..5?

[cnckeith]

In this post I want to attempt to disambiguate the tool references and the tool offsets.

The documentation has many details about manual tool setting but it does not layout start to finish auto tool setting. < Chapter 5 goes over in detail Tool offsets> I will attempt to infer the correct start to finish tool touch off process from the manual process. I don't really know that my guess here is correct and please let me know what the best practices are.

terms:


master tool/reference tool This tool is the reference tool. the best practice is to setup offsets relative to this tool's position. << the offsets are the difference in length between the tools.. not to be confused with some distance relative to a position! the reference position can be anywhere at any given time.. it simply is a way to use the machine as a fancy pair of calipers. as explained in this video..https://youtu.be/4Ik3gFMh8kU>>>

https://youtu.be/4Ik3gFMh8kU


Z ref: The Z ref is relative to WCS Z < no > Z ref should be used to set the position of the master tool. Setting this to part zero is a best practice. < no > there is only one z ref variable but it can be updated for each tool. < what do you mean by z ref variable?> updating the z ref effects all other tool offsets? updating the WCS updates the z ref relative to the WCS change. << you have a basic misunderstanding of Tool Offset values... as explained in the video above offsets are simply the Difference in X and Z Length between tools. nothing more.. the offsets are not relative to some point on the machine!!! as explained in the video you can figure out offsets with a pair of calipers! and then you wouldn't need a Z reference you could set Z zero and run the job! all the tool setup process is using the machine tool as a pair of calipers to figure out how much longer or shorter Tool 2 is from Tool 1 (if you picked Tool 1 as a reference tool) Z reference has nothing to do with running a job it is only used to measure length differences between tools >>>

X diam/X ref: the X ref is relative to WCS X < no > and behaves the same as the Z ref described above. for auto tool setting X ref also should be set to Part zero for the master tool.

tool offset: the tool offset is relative to the Z and X refs. < NO, offsets are relative to the actual reference tool, the reference position is a temporaty postion used at that moment to measure the difference in lenght between tools.>>> the tool offset is kinda double offset from the WCS zero position.

Process 1: initial setup << follow the process shown in the video..>>>

1. chuck the probe and set part X( is this needed?) and Z based on the chucked probe position using m115/m116. The part zero position should be setup with the master tool.
2. enter tool offset menu. manually enter 0.0 for both Z and X ref.
3. manually enter 0.0 for the master tool offsets and tool wear settings.
4. jog away and insert tool to be measured.
5. jog the "slave" tool to a position based on your probe stylus settings.
6. select "measure z and x".

process 2: adding a new tool after initial setup

??? is this the same as the initial setup? << if you haven't powered off the machine and if the Z ref position is still there (you didn't machine it away) then simply go touch the new tool off the reference positions and press the measure button.
now if the reference position is gone..then simply make a new one! it can be any new position since we are simply using it to measure the difference in lenght between the reference tool and the new tool. note no need to remeasure any of the existing tools when measuring a new tool as long as you are using the same Tool 1 as the reference then all the ohter tools are still good to go>>>


Questions:

does setting Z and X refs to 0 simplify auto tool measurement? when would you want to set it to a value other than 0 for auto tool setting?

the manual says x diam is "set for OD". is there an X diam for each tool orientation? is there an x diam for each tool? is there a single variable which should be reset every time you switch from measuring a different orientation or every time you chuck your tool probe? How does this apply to auto tool setting?

why do you need to make a cut for x diam and also another for x offset? This seems redundant? Also this doesn't seem to apply to auto tool setting, should the setting instructions for both x diam and x offset be ignored and just set them to 0 to simplify the setup? <<< don't confuse X0 WCS and the X reference point.. they are not the same point....they can be the same if you want but, in practice they are usually different points on the machine>>>>

How do I check the tool offsets after power down and re-homing? Do I need to run a m6 tool change and then g00 move to a position I can eyeball if the tool offset is correct? << yes, tool change is necessary so the offsets are in place >>

how do you auto set the Z offset for something like a neutral 55 degree tool or a threading tool?

[greenail]

I've updated the first post with what is clarified. Still many things are confusing.

firstly, you say I misunderstand tool offsets because I'm saying they are relative to the WCS. let me be clear in my understanding. the master tool must be relative to the WCS to be positioned correctly. If i setup part zero and jog the master tool to WCS z0 x0 then my tool tip should be at that point. If tool 2 is relative to the master tool then tool 2 must be able to be positioned relative to the current WCS right? If not how does the MCU know where to position the tool during a job? are we getting tripped up on the word "relative"?

< what do you mean by z ref variable?>

there are "Z ref" and "X diam" buttons for each tool but the value is not tied to each tool. I wanted to clarify that.

Next you ask me to watch the video but the video is not using auto tool measuring. How do I know what parts apply and what parts do not? You clearly know your stuff but I don't know it. I have to work through the learning curve. The documentation says to do step 1,2,3 but doesn't explain the why. The video has you measuring all X and then all Z but that doesn't make sense when you should be able to do X and Z in one step with the auto measure routine.

the tool offset is relative to the Z and X refs. < NO, offsets are relative to the actual reference tool, the reference position is a temporaty postion used at that moment to measure the difference in lenght between tools.>>>

maybe it would be more clear to say that the Z/X refs are relative to the tool offset during measurement. Once the offset is measured the Z/X refs are ignored.

you say the z/x ref is not relative to the work coordinate system's X then why does it change when I change the WCS part zero? Should I just ignore part zero entirely when doing auto tool setting?

for adding a new tool I'm assuming the machine has been powered off and the WCS part zero has changed.

"don't confuse X0 WCS and the X reference point.. they are not the same point....they can be the same if you want but, in practice they are usually different points on the machine"

i want to know when they should be the same and when they shouldn't and why that is.

"now if the reference position is gone..then simply make a new one! "

ok so where do I make these new points? you say setting them to 0 is not a best practice. For auto tool setting what is the best practice for setting Z ref and X diam? my probe has a fixed diameter but is not likely to chuck in the same z position. should my first step always be to set the Z ref for the master tool? I don't plan on using paper touchoffs so I'm confused regarding the video's steps.

[greenail]

here is a video of me bumbling through this trying to infer from the official video what to do and gettting a result that does not match up.


https://youtu.be/2WfV05WY-2A

[greenail]

Am I expecting too much to ask to better understand the auto tool measurement feature of the lathe pro software? Is this in the wrong forum?

[Gary Campbell]

Am I expecting too much to ask to better understand the auto tool measurement feature of the lathe pro software? Is this in the wrong forum?

First the easy one. This is the correct forum.

I dont think that you are asking too much, but you need to understand there are numerous ways to accomplish this task, and you may be looking to implement a method that is not familiar or familar enough by most to teach another. Most here have used the above linked videos and manual to get our tool measuring systems up and running. As a CNC instructor myself, I can never predict if a given user will understand my teachings in an hour, a day, a week, or EVER! As humans we all have different cognitive abilities, some simply need to repeat the lesson until it is understood.

I would suggest that you should start with the manual version, get a couple tools measured and verify that they work as expected. Once you have your head wrapped around the process, implement the auto measure version.

[cnckeith]

i agree with gary, as i previously suggested, follow the steps in the video, set up tools manually following the method in the video so you gain a baseline understanding of tool length offsets. then after you have that down..move onto automatic tool measurement. there is no magic in auto tool measurement, the operator still has to understand and adhere to a process which results in determining the difference in length between tools.

[greenail]

I have been able to setup tools via the manual method. I also understand there is more than one way to do it. I am asking for the best practice auto tool setting as well as to help the community by clearly defining the jargon used. I'm happy to write it up but I need to get feedback on it so I can be sure that it is accurate and clear to the users.

You both seem to think that following the steps for manual tool offsets will clarify the process for auto tool setting but it has not and I believe the two reasons are the lack of clear definition for "Z ref"/"X diam" and the fact that the manual directions have you setup all your tools for X, then Z vs X & Z per the auto setting routine.

I will run some tests and create some diagrams, perhaps that will help clarify my questions.

[greenail]

I'd like some feedback on the process and questions below:

Machine is in mm mode

Steps

1. ensure master tool is selected `mdi: T0101`
2. reset zref xdiam and offsets to zero for master tool
3. set part zero for Z and x

Results

WCS: Z0,x0
MCS: Z-114.138 X-39.143

Xdiam and Z diam have changed after setting part zero, Xdiam: -7.986 zref: 0.407


4. auto measure Z ref

Now zref: -0.006

5. auto measure X ref

Now xref: 7.868

6. insert tool 3 and jog to Z,X auto test position

I'm assuming I can manually set the master tool offsets to 0 and that I do not have to run the auto measure routine for Z/X. Is this correct?

7. select tool 3 in offsets screen and run measure Z,X

Tool 3 offsets are now X: 1.227 and z: -4.176


8. turn machine off and rehome.

Next I started centroid back up, rechucked the probe, and set it as part zero to simplify readings.

Part X was off about 0.1mm, I should have written the difference down but the distance should be reflected in the change to "x diam"

Now in Tool offsets my "x diam" is 8.041

Questions:

If xdiam is not relative to the WCS then why did it change when I changed the WCS?

What steps do I use to add or adjust a slave tool? Do I need to remeasure zref and xdiam for the master tool first or do I leave it alone? Do i ever need to run "measuzre z and x" for the master tool?

I can't see any reason not to set the offsets for the master tool to z0 x0 but at one point I ran the auto measure for the master tool and g0z0x0 had it way off and my "x diam" got set to something like 15mm even though the probe is 7.96mm

[cnckeith]

One lathe tool setup method

1.) home machine
2.) set X zero with Tool #1 (x offset = 0 Z offset =0) make a skim cut on scrap material, measure diameter, enter diameter in X part zero setup screen press f10 to save.
3.) Insert probe into spindle
4.) Set up X reference position: highlight Tool #1 X offset (0) and press F1 X diam and choose direction, cycle start to seek probe and set x ref.
5.) Set up Z reference position: highlight Tool #1 Z offset (0) cycle start to seek probe and set x ref.
6.) Tool check and Change Tool to tool #2, jog Tool #2 close to probe
7.) Highlight Tool #2 X offset in tool library.
8.) Measure Tool #2 X offset: Click measure tool, click Measure offset X, choose direction to move to seek probe, cycle start to seek probe, X offset is now entered automatically after successful probing cycle
9.) Measure Tool #2 Z offset: Click measure tool, click Measure offset Z, cycle start to seek probe, Z offset is now entered automatically after successful probing cycle.

Repeat steps 6 thru 9 for all other tools.

Notes:

-offsets are the difference in lenght between Tool #1 and all the other tools. Tool #1 has X and Z offset of 0 since it is not shorter or longer than itself.
-once set the reference position used to measure tool lengths is good as long as you didn't re home the machine, if you re homed the machine you'll have to reset the reference position ONLY if you wish to remeasure or add a new tool to the library.
-once a tool library is set up if you need to add a tool or remeasure an existing tool after re home or power cycle, the reference position will have to be reestablished, no need to remeasure all the tools, just add the new one or reset just one as long as you have the same Tool #1