4 Axis Rotary Feature

Introduction

This help topic lists all of the parameters found in the 4 Axis Rotary Wizard.

Feature 4 Axis Rotary

Rapid Movements

- Clearance Plane - displays the clearance plane value. In the CAM Tree, right-click Machine Setup, and click Edit to set the clearance plane in the Machine Setup dialog box. The clearance plane is incremental from the top of stock (defined in the Stock Wizard). It defines the safe rapid plane used from one feature to the next.
- Rapid Plane - is the height at which the tool can rapid safely within the current machining feature. This value is incremental from the Top of Part setting.
- Feed Plane - is the height at which the tool movement changes from rapid feed rate to feed rate. This value is incremental from the toolpath.
- Top of Part - is the top of the material for the feature. This value is incremental from the Machine Setup or machining origin.
- - Pick Top of Part - enables selection mode for you to set the Top of Part by selecting geometry in the Workspace.

Posting

Posting Parameters

Work Offset # - select the work offset code to use for this feature in the posted NC program. This value defaults to the Work Offset that you selected in the Machine Setup dialog box. The post processor must be configured to support the work offset selected.

Rough Tool

To learn about the tool dialog box, view the Milling Wizard Tool dialog box help topic.

Patterns

Cut Pattern

Zig - sets the cutting method to one-way. All cutting feed moves share the same direction.

Zig Zag - sets the cutting pattern to alternate directions. Each toolpath segment changes cutting direction along the part.

Spiral - (used with Around style only) creates a spiral or ramping cutting pattern along the surface.

Style - defines the general cutting direction of the Rotary toolpath. Select from one of the following options.


Along	Around

Along - creates a toolpath that is parallel to the rotary axis of the part.
Around - creates a toolpath that is normal to or cuts across the rotary axis of the part.

Side Shift - defines a distance that the tool is shifted away from the center of the rotary axis. When a side shift is applied, the tool does not point directly to the rotary axis. This can be used to minimize cutting with the center of the tool.

Rotary Axis

You must select the Rotary Axis being used for the feature. This axis is used for the toolpath creation and is not necessarily the same as the machine's rotary axis. Select the proper axis: X Axis, Y Axis, Z Axis, or User Defined. Notice that when you select an axis, the values that define these directions are updated in the Direction group. When User Defined is selected, type values in the X-, Y-, and Z-boxes to define the custom rotary axis. For example, rotation around the X-axis is defined by the values X1 Y0 Z0. You can also type the X-, Y-, and Z-axis values for the Base Point when the rotary axis is not aligned directly to the X-, Y-, or Z-axis.

Point Tool to Rotary Axis

Select this check box to force the tool axis to point at the defined rotary axis of the part.

Clear this check box to turn off this option.

5th Axis

These options are only available with the 5 Axis Standard, or the 5 Axis Pro modules.

Locked at Angle - is used to lock the 5th axis to a fixed angle.
Relative to Cutting Direction - provides a fixed tilting angle relative to the toolpath cutting direction. This setting forces the Point Tool to Rotary Axis parameter.
- Angle - type the tilt angle for the selected 5th axis parameter.

Cut Direction

You can define the cutting direction as Clockwise or Counterclockwise. This is based on the right-hand rule of the selected rotary axis direction.

Angular Start/End

Cut All - creates a toolpath for the entire part (or geometry selection).
Cut Interval - enables the Angle Start and Angle End parameters for you to define an angular cut interval.
- Angle Start - defines the amount of rotation, from zero degrees, where the toolpath begins.
- Angle End - defines the amount of rotation, from zero degrees, where the toolpath ends.

Parameters

Finish

Stepover - sets the distance between each toolpath segment when using the Around cut pattern.
Step Angle - sets the angular distance between each toolpath segment when using the Along cut pattern.
Allowance XYZ - the distance that the toolpath is calculated from the model geometry. Positive values leave material remaining for a finish pass without having to offset the model geometry.
- Machining Tolerance - the amount of variation allowed for creating toolpaths within the feature. The accuracy of the toolpath does not exceed this range.

Cut Holes - extends the toolpath into any holes that may be present in the surface.
- Ignore Holes - does not place the toolpath into any holes and treats the surface if it is continuous and unbroken.

Limit Along Rotary Axis

These options are used to limit the toolpath to a specific area of the part. When no limit options are defined, the toolpath is applied to the entire selected geometry.

Start

Select this check box to enable the Start setting. Type a value to define the start of the toolpath from the Machine Setup, along the selected Rotary Axis Direction.

Clear this check box when not setting a Start limit.

Start - sets the beginning of the toolpath along the rotary axis. This value is from the Machine Setup or machining origin.

Select this check box to enable the End limit setting. Type a value for the End of the toolpath from the Machine Setup, along the selected Rotary Axis Direction.

Clear this check box when not setting a End limit.

End - sets the end of the toolpath along the rotary axis. This value is from the Machine Setup or machining origin.

Multiple Passes

Select this check box to enable the parameters to create multiple cuts at a defined depth.

Clear this check box to create a toolpath with a single pass (or a single depth cut).

Roughing Passes

Number - is the number of roughing passes applied.
Spacing - is the distance between each pass or the depth of cut.

Finishing Passes

Number - is the number of finishing passes applied.
Spacing - is the distance between each pass or the depth of cut.

Sort by - defines the cutting order for multiple passes.
- Slices - cuts the total depth of each slice before moving on to the next pass.

Passes - cuts the defined depth of each pass before moving to the next pass.

Leads

The Leads dialog box parameters of the Rotary feature are the same as those explained in the 3 Axis Leads dialog box help topic.

Options

Point

Tool Tip - calculates the toolpath from the tool tip.
Tool Center - calculates the toolpath from the center of the bottom of the tool, in the case of a straight cornered end mill, or from the center of the radius on the tool, in the case of bullnose or ball-end mills.

Links

Links

Follow - follows the contour of the surface being machined.

Direct - directly connects one pass to the next with a line.

S-Link - creates a S-shaped link between each path in the toolpath tangent to both paths that lie on the surface of the model.

Filter

Max Link Gap (% of Tool Diameter) - sets the maximum gap between passes, to which it may apply this link type, before retracting the tool. If the distance between the end of one pass and the start of next pass is the same as or smaller than this value, it does not link them. If the distance between the ends of the passes is greater, the tool is retracted to clearance for safety. The value is a percentage of the tool diameter.