Programming of CNC Machines. Ken Evans

ADJUSTING WEAR-OFFSETS FOR TURNING CENTERS

      Wear-Offsets are used to correct the dimensions of the workpiece that change because of cutting tool wear.

      For a Turning Center, the X direction offset corresponds to the diameter, for example: if the X wear offset for a tool is .01, an incremental change of minus .01 refers to a decrease of the diameter by .01 and an incremental change of plus .01 refers to an increase of the diameter by .01.

      To adjust the WEAR-offsets:

      Press the OFFSET/SETTING button until the screen display shown in Figure 38 appears.

       Examples of Adjusting Wear-Offsets

      For the following examples, the operator should display the OFFSET screen for WEAR offsets and the cursor should be positioned to the tool and axis requiring adjustment.

Figure 38 Offset Display Screen for Wear-Offsets

       Example 1: The Absolute System

      If after machining the workpiece shown in Figure 39, the measured external diameter exceeds the value of tolerance (i.e. 1.003), enter the offset with a negative sign assigned to the value -.003 in the wear offset by following these steps.

Figure 39 Examples of a Machine Workpiece used for Adjusting Wear-Offsets

      1. Press X

      2. Key in -.003

      3. Press INPUT

      Then, after machining several more pieces, the diameter increases due to tool wear. If the measured diameter is 1.002, enter the offset as follows:

      1. Press X

      2. Key in -.005

      3. Press INPUT

      Please note that it was necessary to add a value of .002 into the Offset register to the previously entered value of .003. A similar approach is applicable in the direction of the Z axis.

      If the measured length is 1.492, then the value of the offset entered is -.008.

      1. Press Z

      2. Key in -.008

      3. Press INPUT

      A new measured length of 1.494 gives an entered value of the offset of -.006.

      1. Press Z

      2. Key in -.014

      3. Press INPUT

       Example 2: The Incremental System

      To gain a better understanding, let us examine identical cases when the incremental coordinate system is used. The measured value is = 1.003.

      Offset: U

      1. Key in -.003

      2. Press INPUT

      Following that, the diameter is = 1.002.

      1. Press U

      2. Key in -.002 (on the screen)

      3. Press INPUT (X-.005)

      And Z = 1.492

      Offset: W

      1. Key in -.008

      2. Press INPUT

      After machining a few pieces, Z = 1.94.

      Offset: W

      1. Press W

      2. Key in -.006 (on the screen)

      3. Press INPUT (Z-.014)

MACHINING CENTER TOOL OFFSETS

      Tool Length Offsets “TLO” are called in the program by the H-word. The values input into the corresponding TLO# register are needed for proper positioning of the tool along the Z axis. Similarly, the Cutter Diameter Compensation “CDC” values are entered on the Offset display register under column “R” and are called in the program by the D-word. These compensations are important for proper radial (X, Y) positioning of the tool. If the values are known, the following sequence can be used to input them into the offset page. When the setup values are known, you may:

      1. Press the OFFSET/SETTING function key.

      2. Press the OFFSET soft key. It may be necessary to press this key several times until the desired offset display is present.

      3. Use the arrow direction or page keys to position the cursor to the tool number to be set.

      The search method may also be used by entering the tool number whose compensation is to be changed and the pressing the NO.SRH soft key.

      Enter the numerical value of the offset (including sign) and press the INPUT soft key.

      To add or subtract from an existing offset value key in the amount (a negative value to reduce the current value), then press the +INPUT soft key.

      Diameter compensation values are input, as known, after measuring their actual size. Depending on the parameter setting for the specific machine used, the value is entered as either tool diameter or radius. Consult the appropriate manufacturer operation manual for exact conditions.

       Measured Values