CNC Lathe | Tool Offset Registers

In this article, we describe general information about tool offset registration for CNC lathe machines.

0
1081

The word offset with two adjectives – with the expression geometry offset and the expression wear offset. What exactly is an offset? What is the difference between one offset and the other?
On the OFFSET display of a typical Fanuc control, there is a choice of two screens, both very similar in appearance. One is called the Geometry Offset screen, the other is called the Wear Offset screen. Figure 14-9 and Figure 14-10 show examples of both screens, with typical (i.e., reasonable) sample entries (imperial units input).

Geometry Offset

Geometry offset number always matches the turret station number selected. Machine operator measures and enters geometry offsets for all tools used in the program.

GEOMETRY offset amount is always measured from the machine zero position!

Distance from machine zero position will reflect the distance from tool reference point to part reference point (program zero). Figure 14-11 shows a typical measurement of geometry offset applied to a common external tool.

You may be interested also “CNC Lathe | G70 Cycle | Contour Finishing”

All X settings will normally have diameter values and are stored as negative for a typical rear lathe of a slant bed type. Z-axis settings will normally be also negative (positive values are possible but impractical). How to actually measure geometry offset is a subject of CNC machine tool operation training, not programming. Manual and automatic methods are available for this purpose.
Figure 14-12 shows a typical measurement of geometry offset applied to a common internal tool.

One last possibility relating to geometry offset is illustrated in Figure 14-13. It shows geometry offset applied to any tool used on the spindle center line (always at X0 position). These tools include center drills, drills, taps, reamers, etc. Their X-offset setting will always be the same.

Wear Offset

In CNC program development, many dimensions used will be those in the part drawing. For example, a dimension of 3.0000 inches, is programmed as X3.0. This figure does not reflect any implied dimensional tolerances. Program entries X3.0, X3.00, X3.000 and X3.0000 have exactly the same result.What is needed to maintain dimensional tolerances, particularly when they are tight? What has to be done with a worn out tool that is still good enough to cut a few more parts? The answer is that the programmed tool path must be adjusted, fine-tuned, to match the machining conditions. Program itself will not be changed, but a wear offset for the selected tool is applied.

WEAR offset amount is the difference between programmed value and the actual measured size of part!

Figure 14-14 illustrates the principle of tool wear offset, although the scale is exaggerated for emphasis.

Figure 14-14
Programmed tool path and tool path with wear offset

Actual wear offset setting has only one purpose – it compensates between the programmed value, for example that of dia 3.0 inch, and the actual dimension as measured during inspection, for example, dia 3.004. The differential value of -0.004 is entered into the wear offset register. This is the offset number specified as the second pair of tool function used in the program. Since the program uses diameters for the X-axis, offsets will also be applied to diameter. Details on this kind of adjustment are more useful to CNC machine operator, but any part programmer will benefit from them as well.

Wear Offset Adjustment

To illustrate the concept of wear offset adjustment on a rear type lathe, T0404 in the program will be used as an example. The goal is to achieve an outside diameter of 3.0 inches and tolerance of 0.0005. Initial setting of the wear offset in register Txx04 will be zero. Relevant section of the program may look something like this:
N31 M01

N32 T0400 M42
N33 G96 S450 M03
N34 G00 G42 X3.0 Z0.1 T0404 M08
N35 G01 Z-1.5 F0.012
N36 …
When the machined part is inspected (measured), it can have only one of three possible inspection results:

  • On-size dimension
  • Oversize dimension
  • Undersize dimension

If the part is measured on size, there is no need to interfere. Both tool setup and program are working correctly. If the part is oversize, it can usually be recut, if machining an outside diameter. For an inside diameter, the exact opposite will apply. Recut may damage the surface finish, which should be a concern. If the part is undersize, it becomes a scrap. The aim is to prevent all subsequent parts from being undersize as well. The following table shows inspection results for all three existing possibilities:

Let’s go a little further.Whether the part will be oversized or undersized, something has to be done to prevent this problem from happening again. Common action to take is adjusting the wear offset amount.Again, the emphasis here is that this is an example of an outside diameter.
External diameter X3.0 in the example may result in 3.004 diameter measured size. That means it is 0.004 oversize – on diameter. CNC operator, who is in charge of offset  adjustments, will change the currently set 0.0000 value in the X-register of the wear offset 04 to -0.0040. The subsequent cut should result in a part that will be measured within specified tolerances.
If the part in the example is undersize, say at 2.9990 inches, the wear offset must be adjusted by +0.0010 in the X-positive direction. Measured part is a scrap.
Principle of the wear offset adjustment is logical. If the machined diameter is larger then the drawing dimension allows, the wear offset is changed into the minus direction, towards the spindle center line, and vice versa. This principle applies equally to external and internal diameters. The only practical difference is that an oversized external diameter and undersize internal diameter can be recut (see the table above).

The R and T Settings

The last items are the R and T columns (Geometry and Wear). Both offset screen columns are only useful during setup. The R column is the radius column, T column is the tool tip orientation column (Figure 14-15).

Figure 14-15
Arbitrary tool tip orientation numbers used with tool nose radius
compensation (G41 or G42 mode)

The main rule of using R and T columns is that they are only effective in tool nose radius offset mode. If no G41 or G42 is programmed, settings in these two columns are irrelevant. If G41/G42 command is used, non-zero values for that tool must be set in both columns. The R-column requires tool nose radius of the cutting tool, the T-column requires tool tip orientation number of the cutting tool.
Tool tip numbers are arbitrary and indicate the tool orientation number used to calculate the nose radius offset, regardless of tool setting in the turret.


Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleCNC | G09 and G61 Codes | Exact Stop
Next articleCNC | G54-G59 Codes | Work Offsets