CNC Services Northwest

Method 1b: Use a common tool from many jobs as a reference tool for both axes

Use this method if you want to have a clear visual illustration of your offset values, and you have a tool which you use on many jobs and rarely change.

Pros:

No need for a separate, dedicated reference tool
Can measure tools off of any convenient surface

Cons:

Must measure every tool if the reference tool is changed.

Preparation (whenever the reference tool is changed)

This procedure will set the X axis part position based on the reference tool. All other tools will have X tool offsets relative to the reference tool.

Load the tool you wish to use as a reference tool.
Go to X axis Part Setup (F1/Setup, F1/Part, F8/X axis).
Using manual controls, turn a true-running diameter on some stock.
Move the tool clear in the Z+ direction, but do not move it in X yet.
Measure the turned diameter.
Enter Position=measured diameter, Tool=0, Set All WCS=Yes.
Press F10/Set.
Press ESC three times to return to the main screen.

Operation (for each job)

Load all of the tools for the job into their tool holders.
Load the tool you wish to use as a reference tool into the tool post.
Go to Z axis Part Setup (F1/Setup, F1/Part).
Using manual controls, turn a clean face on the stock.
Without moving the tool away from the face, enter Position=0, Tool=0.
Press F10/Set to set Z zero here.
Press ESC to return to the Setup screen.
Press F2/Tool Offset to go to the Tool Offset Library.
Press F2/Measure Tool to access the tool-measuring functions.
Verify that the X Offset and Z Offset values for the tool that you are using as a reference tool are both zero.
Jog the reference tool to touch the end face of the stock (if it is not already there from the previous step).
Use the right or left arrow keys to move the highlight into the "Z Offset" column, on any line.
Press F1/Z Ref.
Press F10/Set to set the Z axis tool-measuring reference position here
Using manual controls, turn a true-running diameter on the stock.
Move the tool clear in the Z+ direction, but do not move it in X yet.
Use the right or left arrow keys to move the highlight into the "X Offset" column, on any line.
Press F1/X Diam.
Press F10/Set to set the X axis tool-measuring reference diameter here.
For each remaining OD tool:
1. Arrow up or down to highlight that tool number in the library.
2. Load the tool onto the tool post.
3. Jog to touch off on the outside diameter of the stock.
4. Press F5/Measure Offset X to measure the tool's X offset.
5. Press F10/Measure to measure the tool at the current position.
6. Jog the tool around to touch the end face of the stock.
7. Press F6/Measure Offset Z to measure the tool's Z offset.
8. Press F10/Measure to measure the tool at the current position.
If you have ID tools to measure, which can be touched off to an inside diameter on the front (X+) side of the spindle centerline:
Arrow left or right to the "X Offset" column.
Press F1/X Diam to set a new X Reference. Following the second set of instructions:
1. Type the measured diameter of the inside of the bore, as a positive number.
2. Press F10/Set to set the X axis tool-measuring reference to the entered value.
Arrow right to highlight any Z offset
Press F1 to set Z Reference. Following the instructions:
1. Jog to touch off on some convenient surface (e.g. the end of the part).
2. Press F10 to set Z Reference here.
For each ID tool which can be measured in the front of the bore:
1. Arrow up or down to highlight that tool number in the library.
2. Load the tool.
3. Jog to touch off on the inside diameter.
4. Press F5/Measure Offset X.
5. Press F10/Measure to measure the tool's X offset here.
6. Jog around to touch off on the end (Z) surface.
7. Press F6/Measure Offset Z.
8. Press F10/Measure to measure the tool's Z offset here.
When all tools have been measured, Press F10/Save to save the measured offsets.
Press to return to the main screen.

If you have to replace one tool

Go to the Offset Library
If the surfaces you measured the tools on before are still available (i.e. have not been machined away) then you do not have to reset the X and Z Reference positions.
If the previous surface is not available, load the reference tool and set X and Z References on a new surface, using the same procedure you used before.
If the tool to be measured is an ID tool, then type in the X reference diameter, instead of touching it with the reference tool.
Load the new tool and measure both X and Z offsets off the same surfaces.

Notes

When measuring a replacement tool, you do not have to use the same surfaces you used to measure the other tools, as long as you reset the References off of the new surface before measuring the new tool.

Before measuring a tool's X offset with F5/Measure Offset X, you need to make sure that the "X Diam" value in the lower left corner shows the diameter that the new tool's tip is currently at or touching.

There are two ways to set that "X Diam" reference value:

You can teach it by example, by touching that diameter with the reference tool.
You can measure the diameter and type it in.

There are several ways to measure the X offset for an ID or back-side tool:

You can touch the tool to the back side of a straight edge, held against the front (OD) of the stock.
In this case, the reference X Diam would be positive, and probably the same as what you used for OD tools.
You can touch the tool inside an ID bore, again on the front (X+) side of spindle centerline.
In this case, the reference X Diam would be positive, equal to the measured ID.
You can touch the tool to the outside diameter on the back (X-) side of the stock.
In this case, the reference X Diam would be negative: equal to the measured OD but with a minus sign.

Note that there is a bug in CNC12 Lathe software, at least through version 4.20, which causes tools with "Tool Orient" = "ID" and "Tool Type" = "Thread" to be measured incorrectly. To get correct X offset measurements for an ID threading tool, you should set its "Tool Type" to "Turn" instead.