Patterns

Introduction

This topic explains the Patterns page of the Equidistant operation found in the Mill 3 Axis Wizard.

Patterns

Cut Pattern

When creating Equidistant operations, you have two options to determine how the equidistant offset is created. You can select the feature geometry without selecting Drive Curves and the software automatically creates the offset pattern (using the boundary of the model), or you can select Drive Curve geometry in addition to the feature geometry to determine how the offset pattern is created.

 

  • Pick Drive Curves

    Select the check box when you want to assign a Drive Curve to the Equidistant operation. Click Pick Drive Curves to select the drive curve geometry, and confirm your selections to return to the wizard. You can select one or more open or closed chains that are used to generate the offsets for the operation. The result is a morph style toolpath.

    Clear the check box when you want to create the standard equidistant operation without selecting any Drive Curves. (The software automatically uses the boundary of the feature to create the offset pattern.)

 

Note: You do not have to select Drive Curves to use the Step Direction and Number of Cuts parameters.

 

Drive Curves

 

  • Step Direction - determines the direction in which the toolpath is applied from the Drive Curves, when selected, or when no Drive Curves are selected, from the boundary of the operation. The direction is determined by the chain-direction of the selected Drive Curve. When no Drive Curves are selected, the software automatically applies the direction to the boundary of the operation. This option is then used in combination with the Number of Cuts.

    • Left - creates the operation to the left side of the chain direction.

      Left

    • Right - creates the operation to the right of the chain direction.

      Right

    • Both - creates the operation on both sides of the drive curves or boundary.

      Both

 

Tip: When defining multiple Drive Curves, the Drive Curve that covers the largest area is used to determine the chain direction used for the Number of Cuts parameters. To make it easier to create the desired result, you should set all Drive Curves to use the same general chain direction and then adjust the wizard parameters to create the desired result.

 

  • Number of Cuts Left - defines the number of passes that are created to the left side of the selected Drive Curves (or the boundary of the operation) when using Step Direction Left or Both.

  • Number of Cuts Right - defines the number of passes that are created to the right side of the selected Drive Curves (or the boundary of the operation) when using Step Direction Right or Both.

     

Important: When the Number of Cuts parameters are set to zero, the operation is applied to the entire model or boundary. When greater than zero, the software always creates a pass on the Drive Curve (or boundary) plus the value specified for the Number of Cuts parameters. For example, when selecting Drive Curves and setting the Number of Cuts to two, three passes are created.

 

Number of Cuts

 

For example results of the previous parameters, view Equidistant Examples.

Method

  • Zig - creates the operation so each pass of the tool follows the same general direction (one way machining).

 

Zig

 

  • Zig Zag - creates the operation so each pass of the tool alternates direction from the previous pass.

 

Zig Zag

 

  • Spiral - creates the operation so the tool travels in a spiral motion around the part.

 

Spiral

 

 

 

Cut Direction

  • Climb Mill - the tool travels in a counter clockwise direction along the inside shapes of the model and travels in a clockwise direction along the outside edges of the model.

  • Conventional Mill - the tool travels in a clockwise direction along the inside shapes of the model and travels in a counter clockwise direction along the outside edges of the model.

 

 

Start Location

 

- With this check box cleared, the Start Location group will be empty, and the operation will begin in its default location.

 

- With this check box selected, the Start Location group will be available, giving you the ability to set start location of the operation.

 

  • Pick - closes the wizard, and launches the Pick Start Location dialog in the Property Manager, to allow you to select a point, or vertex to set as the start of the operation. Select the point, and click OK. The wizard returns and the coordinates of the selected point is populated in the X, Y, and Z text boxes.

    • X - allows you to manually set, or adjust the start point of the operation along the X axis.

    • Y - allows you to manually set, or adjust the start point of the operation along the Y axis.

    • Z - allows you to manually set, or adjust the start point of the operation along the Z axis.

 

 

Sorting

  • Standard - machining starts from the outer most loop on the part and progresses inwards.

  • Center Away - machining starts from the inside and progresses outwards within each region.

  • Outside to Center - machining starts from the outside and progresses inwards within each region.

  • Top to Bottom - machining starts at the top slice for all regions.

  • Bottom to Top - machining starts at the floor for all regions.