Method 1a: Use a centerline tool as the reference tool for X, any tool for Z
Use this method if you want to have a clear visual illustration
of your offset values.
Pros:
Easy to visualize offset values
All centerline tools have X offset of zero
The X axis offset value for each tool will be the distance between that
tool tip and the center of an ID tool holder, expressed as a diameter
(i.e. the offset will be 2x the actual distance).
The Z axis offset value for each tool will be the distance between that
tool tip and the tip of whatever tool you choose as the reference tool
for the Z axis.
The reference tool for the Z axis does not need to be a centerline or
ID tool. Most people use a common OD turning tool for this purpose.
You could also use the face of the turret or the face of a tool holder,
instead of an actual tool.
Preparation (one-time)
This procedure will set the X axis part zero position based on a
centerline tool holder.
Using either a test indicator in the chuck, or a piece of
smooth and true-running bar stock that matches the ID
of one of your centerline tool holders, jog the X axis
until the centerline tool holder is exactly aligned with
the spindle centerline.
Go to X axis Part Setup (F1/Setup, F1/Part, F8/X axis).
Enter Position=0.0, Tool=0, Set All WCS=Yes.
Press F10 to set.
Operation (for each job)
Load all the tools into their holders.
Index the turret to the tool you want to use as a reference on the Z axis.
Put a piece of stock of known diameter in the chuck or collet.
Go to Z axis Part Setup (F1/Setup, F1/Part).
Jog the tool in to touch the end of the stock. Face the
stock if needed to get a smooth surface.
Enter Position=0.0, Tool=0 (regardless of the actual tool number).
Press F10/Set to set Z zero here.
Without moving the tool, go to the Offset Library (ESC, F2/Tool, F1/Offsets).
With any Z Offset highlighted, press F1 to set Z Reference.
Press F10/Set to set Z Reference here.
If the tool you are using for Z reference is an actual, numbered tool,
then highlight its Z Offset
and press F2/Measure. The resulting offset measurement should
be 0.0 (this is the reference tool, so it has zero offset).
Now jog around to touch an outside diameter.
If the stock runs true, just touch the tool to the stock.
If the stock does not run true, use the jog keys to take light
turning cuts until it does run true, then, without moving the
X axis from the final cut position, mic the resulting diameter.
With any X Offset highlighted, press F1 to set X Reference.
Type the stock diameter into the box and press F10.
Highlight the X Offset for this tool and press F2/Measure.
The resulting offset will generally not be zero.
For each remaining tool:
Load the tool.
Highlight the X Offset for that tool number.
If it is a centerline tool (drill, tap, etc.),
just type 0.0 and press Enter.
If it is an off-center ID tool (boring bar), type in
the calculated offset and press Enter (see below).
If it is an OD tool:
Jog to touch off on the outside diameter.
Press F2 to measure the X Offset.
Now highlight the Z Offset for that tool number.
Jog to touch off on the end of the stock.
Press F2 to measure the Z Offset.
Press F10 to save the measured offsets.
For Centerline and ID tools, you do not have to touch off and measure X offsets.
Instead, you can enter known offsets.
Any centerline tool (e.g. center drill, drill, tap, reamer) will have an
X offset of 0.0.
Boring bars will have an X offset based on the Center Line distance (the
distance from the boring bar centerline to the cutting edge). Generally
the cutting edge will point in the X+ direction (so the ID boring tools
cut using the same spindle rotation as the OD turning tools). In that
case, the X offset for a boring tool will be negative 2x the Center Line
distance. E.g. a boring bar with a Center Line distance of 0.250" will
have an X offset of -0.500".
The Center Line distance for a given boring bar is usually given in the
tool supplier's catalog.
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 Z surface is not available, index to the reference tool and
set Z Reference on a new surface, using the same procedure you
used before.
If you need to set up an OD tool and the previous X surface is not
available, then measure a new turned surface
and enter the measured value as the X Reference Diameter.
Load the new tool, measure or enter the X offset, and measure the Z offset
as you did before.
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.
