Technology page

This page enables you to define the technological parameters of the machining.

Mode

This section enables you to choose the side of the machining. The Front and Back options enable you to perform facial turning on front and back faces, respectively.

Working area 

This section enables you to define where the face turning will be started.

  • Stock

When this option is chosen, machining starts at the stock boundary. The maximal (if Front is chosen for Mode) or minimal (if Back is chosen for Mode) Z-coordinate of the stock is automatically determined. The cutting passes parallel to the X-axis are distributed between this coordinate and the geometry.

  • Target extended by

When this option is chosen, machining starts at the offset from the target defined in the corresponding edit box.

Direction

This section defines the direction of the tool movements.

  • One way

The tool path passes are performed only in the direction of the geometry; the tool returns to the starting point of the next pass in the Rapid mode (G0) outside of the material.

  • Zigzag

The tool path passes are performed both in the direction of the geometry and in the reverse direction. After reaching the end of the first pass, the tool performs the next pass in the opposite direction, and so forth.

Rough

This section enables you to perform rough face turning. The roughing is performed in a number of cutting passes parallel to the geometry. The distance between two successive cutting passes is defined by the Equal step over parameter.

Rough type

This section enables you to define the type of roughing.

  

  • Smooth

At the end of every pass, the tool continues moving along the geometry until it meets the previous pass; then it retreats from the material. A smooth material boundary results from this type of turning.

  • Stairs

At the end of every pass, the tool retreats away from the material. A stairs-shaped material boundary results from this type of turning.

 

Final steps

This option enables you to divide the machined area into two regions, each with its own Step over, when the Step over of the region closer to the final machining surface is smaller.

The Number of cuts value defines the number of final cuts.

The Step over value defines the distance between two successive final cuts.

  

Offset

This section enables you to define the offset along the Z-axis that will remain unmachined during the roughing, i.e. the allowance for the further finishing.

More

  1. Rough offset

  1. This parameter is available only when the Rough section is activated.

Retreat distance 

This parameter enables you to define the distance to which the tool retracts after each cutting pass in case of One way machining. The retract movement is performed along the Z-axis over the cutting level. Then the tool moves parallel to the X-axis to the start point of the next cutting pass; the movement is performed in the Rapid mode. Then the tool descends along the Z-axis to the next cutting level and continues the machining.

  1. This parameter is available only when One way is chosen for Direction.

Use cycle

This option enables you to define whether the turning cycles of the CNC-machine will be used (the check box is selected) or the tool path movements will be generated by SolidCAM (the check box is not selected).

  • When this check box is selected, SolidCAM updates the geometry according to the tool shape and generates the GCode for the CNC-controller cycle including the parameters required to execute the cycle and the GCode of the updated geometry.

  		•

    In this case, the simulation might be slightly different from the actual machine cycle.

  • When this check box is not selected, SolidCAM updates the geometry according to the tool shape and then calculates the minimum tool movements required taking into account the material boundary in the beginning of the operation.

With rapid

When this check box is selected, the tool approaches the material at each Step over in the Rapid mode.

Finish

When this check box is selected, a single finishing pass is performed in the end of the operation.

Compensation

This option enables you to use the compensation of the tool nose radius.

  • When this check box is not selected, the radius of the tool nose is not taken into account when calculating the tool movements. No tool nose radius compensation (G41/G42) is used in the GCode.

  • When this check box is selected, the radius of the tool nose is not taken into account when calculating the tool movements. However, the tool nose radius compensation (G41/G42) is used in the GCode.

X output

The Negative X output option enables you to perform turning in the negative direction of the X-axis. The tool mounting and offset should be chosen accordingly.

  		1.

    The offset for the negative X output is applied to the absolute dimension on the X-axis.

 

Related Topics

  1. Face Turning Operation
  2. Facial turning