Data

When the Technology Wizard is in the iMachining Operation dialog box, the Feed and Spin data for the tool are automatically calculated according to the selected set of Cutting conditions. When GCode is generated, the corresponding Data is written to the GCode file.

This tab displays the individual Feed and Spin parameters for the current operation.

The Feed values can be displayed in the following two types of units:

  • F is the default type displaying units of distance per time.
  • FZ displays the equivalent values in units of distance per tooth, which are calculated according to the formula FZ = F/(Number of flutes × S).

The Spin values are displayed in the following two types of units:

  • S is the default type displaying revolutions per minute.

  • V displays the equivalent values for material cutting speed (velocity between the edge of the cutting tool and the surface of the workpiece), which are calculated according to the formula V = (S × π × Diameter)/1000 for Metric units and V = (S × π × Diameter)/12 for English units.

Feed

By default, the following feed rates are automatically calculated for the tool:

  • Feed XY – this value sets the feed rate for when the tool is cutting at maximum Step over. This feed rate is also the slowest feed rate when cutting.
  • Feed XY max – this value sets the maximum cutting feed rate. This feed rate can be used to limit the entire cutting feed rate by overriding the Feed XY value.
  • Finish feed XY – this value sets the finish feed rate when using iRough + iFinish or iFinish, where the finish pass uses a separate feed rate.
  • Feed Z – this value sets the feed rate for the Z-down movements and the helical reposition moves when down in the cut.
  • Feed helical – this value sets the feed rate for the helical entry.
  • Feed reposition – this value sets the feed rate for reposition moves when the Z is down in the cut.
  • Finish feed floor – this value sets the finish feed rate when finishing the floor with the Contour style tool path only.

Spin

By default, the following spindle speeds are automatically calculated for the tool:

  • Spin rate – this value sets the maximum spindle speed for when the tool is cutting in XY.
  • Spin finish – this value sets the finish spindle speed when using iRough + iFinish or iFinish, where the finish pass uses a separate spin rate.
  • Spin helical – this value sets the spindle speed for the helical entry.
  • Spin floor – this value sets the finish spindle speed when finishing the floor with the Contour style tool path only.

Gears

If the drive system of your CNC-Machine has two or more gears with different spin limitations, they can be individually defined in the VMID's Drive Unit settings. When more than one is defined, you can select your preferred gear for use in the operation from the Gear list. By default, the gear is automatically selected according to each of the Spin values. Only gears having the current Spin value within their range are shown in the list.

The first parameter enclosed in parentheses indicates the defined spin range; the second parameter indicates the defined power.

Overriding parameters

Override check boxes are available for most parameters, but Feed XY and Spin rate are shown with a icon because they need to be synchronized when using the Wizard. If you want to manually enter preferred values for the locked parameters, the Wizard can be turned to open the fields for editing.

When using the iMachining technology, it is highly recommended to leave the Wizard On and utilize the optimal feed rates and spindle speeds that are provided. The Wizard automatically calculates these values according to many factors.

If you override a parameter by selecting its check box , use of the Machining level slider will have no effect on the corresponding value.

Offsets

Length offset number – this parameter defines the number of the Length Offset Register of the current tool in the Offset table of the CNC-Machine.