The Utility Tab

Introduction

The Utility tab of the Multiaxis Wizard contains the following parameters.

Feedrate Control

  • Surface Radius Based Feed Optimization
    Select the check box to use feedrate optimization for any surface with a radius. To define the setting in the Surface Radius Based Feedrate Optimization dialog box, after selecting the check box, click .
    Clear the check box to turn off this option.

    The Surface Radius Based Feedrate Optimization dialog box allows you to set different feed rates for four different radius values: two are user defined, one is for flat surfaces, and the last is for no radius. Type a radius value for each user defined radius. Type a percentage of the feedrate to use for each defined radius.

  • Tool contact based feed rate optimization
    Select the check box to turn on the Tool contact based feed rate optimization option which allows you to specify a minimum percentage of feedrate. To define the parameters in the Feed Control Zone dialog box, after selecting the check box, click .
    Clear the check box to turn off the option.

  • Feed control zone
    Select the check box to turn on the feed control zone option which allows you to specify a geometric boundary as an area to apply a special feedrate. To define the parameters in the Feed Control Zone dialog box, after selecting the check box, click .
    Clear the check box to turn off the option.

    Feed Control Zone Dialog Box
    • Geometry - click to select geometry as the boundary area for feedrate control.
    • Offset - type a positive value here to offset the boundary area from the selected geometry thus making the feed control zone smaller.
    • Inside feedrate % - type a percentage of the feedrate that is applied inside of the feed control zone.
    • Outside feedrate - type a percentage of the feedrate that is applied outside of the feed control zone.

  • Use rapid feedrate
    Select the check box to use rapid feedrate and type the desired rapid feedrate value in the box.
    Clear the check box to turn off rapid feedrate. Retract moves, for example, now use the standard feedrate.

  • First cut feedrate % - allows you to specify a percentage of the normal feedrate applied to the first cut of the toolpath. A setting of 100 means that the normal feedrate is used and the first-cut feed rate is not changed.

This section allows for control over the feedrate for direct, or blend spline links.

 

  • Gaps along cut - when the direct, or blend spline links are used for the Gaps along cut, select the check box and enter the desired feedrate.

  • Links between slices - when the direct, or blend spline links are used for the Links between slices, select the check box and enter the desired feedrate.

  • Links between passes - when the direct, or blend spline links are used for the Links between passes, select the check box and enter the desired feedrate.

Axial Shift

The Axial Shift parameter is an offset applied to the tool along its axis. The result is that different parts of the flute are used for cutting at different parts of the toolpath. The Axial Shift section of the Utility tab is described next.

 

You can select one of the following options for an axial shift.

 

  • Constant for Each Contour - applies a constant axial shift to the tool for each toolpath contour. In the following image, (1) shows the axial shift distance (To value) is constant at each toolpath contour (2).

 

 

 

  • Gradual for All Cuts - applies an axial shift gradually (using the From and To distance values) for each new cut. The result is that a different part of the tool is used for each new cut. The following image shows (1) the Fromdistance value, (2) the To distance value, and (3) each cut.

 

 

 

  • Gradual for Each Contour - applies an axial shift gradually (using the From and To distance values) for each new toolpath contour. The result is that a different part of the tool is used for each new contour. The following image shows (1) the From distance value, (2) the To distance value, and (3) the starting contour.

 

 

 

After selecting an option, you must set the distance values for the axial shift. When using Constant for Each Contour, only the To distance value is available since the shift is constant.

 

  • To - type the axial shift distance for the beginning of the toolpath.

  • From - type the axial shift distance for the end of the toolpath.

 

Note: Positive values cause the tool to retract and negative values cause the tool to plunge (in-feed).

 

  • Damp

Select this check box to apply damping to the axial shift. Damping is used to reduce sudden tool shift movements.

Clear the check box to turn off damping.

Miscellaneous

  • Max. Angle Step for Rotation Axis
    This option determines the maximum angle step, or amount or rotation, applied to rotation axis movements between toolpath points. Select the check box to turn on the option and then type the angle value in the box. Any machine movement beyond this angle is reduced by adding more toolpath points to smoothen the machine movements as a division of the angle change and maximum angle step. This is provided to reduce or eliminate abrupt machine movements, specifically for some machine controllers that do not limit large rotation changes, which can break tools or gouge surfaces.

  • Set Y-axis Machine Limits - for special case machining (turbine blades), this option allows you to limit the Y-axis machine movement.
    Select this check box to turn on Y-axis machine limits. Type values in the boxes to set the minimum and maximum Y-axis machine limits.
    Clear this check box to turn off Y-axis machine limit.

  • Smooth Surface Normals - helps to minimize abrupt tool movements that result from large changes in surface normal direction along a toolpath.
    Select the check box to smooth surface normals. Type a value in degrees to set the maximum angle change allowed between surface normals (along a toolpath). Any change greater than this value is smoothed.
    Clear the check box to turn off Smooth surface normals.

  • Calculation Based on Tool Center
    Select the check box to use calculations based on the tool center.
    Clear the check box to use calculations based on the tool tip.

Example

The following image shows calculations based on tool tip (surface contact point).

 

 

 

The following image shows calculations based on tool center.

 

Markers

The Markers group provides options to alter the output of the program specifically for laser machining. The following options are provided to mark the output of sharp corners or lead-in moves so that, for example, you can lower the power setting of the machine during these moves.

 

  • Sharp Corners

Select the check box to enable the Distance to Corner and Corner Detection Angle parameters used to mark sharp corners in the toolpath.

Clear the check box when you are not marking sharp corners.

    • Distance to Corner - sets the distance from a sharp corner that the marker is applied.

    • Corner Detection Angle - sets the angle at which a change in the toolpath is considered a sharp corner.

  • Lead-in

Select the check box to mark lead-in moves at a specific distance from the toolpath/contour.

Clear the check box when not marking lead-in moves.

    • Distance to Contour - specifies the distance from the toolpath contour that the lead-in move is marked.

Related Topics

The Multiaxis Wizard