Hole Geometry Selection

This section explains how to select geometry for  Drill, Tap, Counterbore, and Thread features. This information applies to standard hole drilling, multiaxis drilling, and cross drilling.

Geometry Selection

To access the Selection Manager for hole geometry, do one of the following:

• In the Hole Wizard, click Select Geometry.
  
  
• Under a Hole feature in the CAM Tree, right-click Geometry and click Re/Select.

The Hole Geometry Picking dialog displays in the Data Entry Manager:

Supported Geometry Types

When selecting geometry for drilling features, you can select points, arcs, lines, surface edges, or cylindrical surfaces. All drilling types support all of these geometry selections, with one exception that points cannot be selected for multiaxis drilling.

Drill Holes Example Part

Supported Geometry Selections

The following images show all supported geometry selections that can be used to for the example part.

Points	Arcs	Lines

Surface Edges (Top or Bottom)		Cylindrical Surfaces

Important Notes About Geometry Selection

Benefits of Cylindrical Surfaces

Selecting cylindrical surfaces allows the software to automatically set the diameter, top of feature, and the feature depth for you. You must manually set one or more of these values when using any other geometry type.

Benefits of Lines

Selecting lines allows the software to automatically set the top of feature and the feature depth for you. Note that you must type the diameter value in the wizard.

Points, Arcs, or Surface Edges

Depending on the Z-axis location of the geometry and the settings that you define, the software may automatically set the diameter, top of feature, or feature depth, but not all of them. Be sure to properly set (or confirm) all of these parameters when using these geometry types.

Multiaxis Drilling

Points cannot be selected for multiaxis drilling (as no direction can be determined from a point).

Geometry Filtering

The software automatically filters the geometry selections you make in a few ways. First, the software attempts to remove all extra geometry, for example, duplicates or concentric entities. Second, the software filters the selections you make, based on the drilling type and hole/tool orientation, to remove holes with orientations that are incorrect for the selected drilling type.

Important: If you find that the geometry you select for drill holes is being removed by the software, confirm that you are selecting the appropriate geometry for the drilling type. For example, with standard drilling, a hole that isn't parallel to the Z-axis is removed because it would require multiaxis drilling.

Hole Type

The first part of using the Selection Manager is to select the type of drilling you are performing: Standard, Multiaxis, or Cross Drill (for Mill Turn only). The software automatically filters the geometry that you select to only include holes (tool orientations) that can be drilled using the selected type.

Tip: The drilling type that you select during hole geometry selection determines the type of feature that you are creating: Standard, Multiaxis, or Cross Drilling. The geometry that you select is automatically filtered to remove orientations that do not apply to the selected drilling type and machining origin coordinate system. [The filtering happens when you confirm (OK) the selection.]

• Standard Drill
  Standard drilling, the default drilling type, is used when the tool orientation to drill the holes is parallel to the main spindle direction, usually the Z-axis. This includes face drilling for Mill Turn jobs. Standard drilling may also be used with index systems, for example, with 3x2 machining on a 5-axis machine where you index to a plane and then perform 3-axis machining (although multiaxis drilling eliminates the need to create index systems).
  
  Mill or Mill Turn Standard Drilling
  The following images show toolpath examples of standard drilling for both Mill and Mill Turn jobs.

Mill Standard Drilling	Mill Turn Standard Drilling

• Multiaxis Drill
  Multiaxis drilling is used for multiaxis machining (more than three axes), in which the tool orientation may or may not be parallel to the main spindle direction. This drilling type is also used for Mill Turn jobs, for example, when drilling holes on the circumference where the tool orientation does not point to (or cross) the rotation axis of the part (usually the Z-axis).
  
  Mill or Mill Turn Multiaxis Drilling
  The following images show some example multiaxis toolpath. Note that Multiaxis drilling can also perform standard drilling.

Mill Multiaxis Drilling	Mill Turn Multiaxis Drilling

• Cross Drill
  Cross drilling is only available for Mill Turn jobs, which may be called diameter or radial drilling. This drilling type is used when the tool orientation points directly to, or crosses, the rotation axis of the part, usually the Z-axis. Note that the tool orientation must also be perpendicular (at a right angle) to the rotation axis. On the physical machine, the tool orientation for cross drill holes is parallel to the X-axis.
  
  Mill Turn Cross Drilling
  The following images show example cross drilling toolpath. Note that cross drilling does not require Y-axis capabilities. Drill holes that require Y-axis movement are not considered cross (radial) drilling and are handled using Multiaxis drilling.

Mill Turn Cross Drilling

Point and Arc Usage

These options determine how the software calculates the toolpath when selecting points, arcs, or surface edges for hole geometry. The parameters that display in the Selection Manager change slightly for each drilling type as explained next.

Standard Drill

After selecting Standard Drill, the following options become available.

• Ignore Z - means that the Z-axis location of the geometry is ignored so that you can manually set the Top of Feature and the Feature Depth in the wizard. This option is helpful when the selected geometry is not the top or bottom of the hole.
  
  
  
  
• Use as Top - means that the geometry is the Top of Feature (the top of the hole). The software calculates the toolpath using the Z-axis location of the geometry as the top.
  
  
  
  
• Use as Bottom - means that the geometry is the bottom of the feature (bottom of the hole). The software calculates the toolpath using the Z-axis location of the geometry as the bottom.
  
  
  

Multiaxis

After selecting Multiaxis, the following options become available.

• Use as Top - means that the geometry is the Top of Feature (the top of the hole). The software calculates the Top of Feature using the Z-axis location of the geometry.
  
  
  
  
• Use as Bottom - means that the geometry is the bottom of the feature (bottom of the hole). The software calculates the Top of Feature using the Z-axis location of the geometry.
  
  

Drilling Direction and Removing Individual Holes

When selecting geometry for multiaxis, each hole contains a drilling direction, which is indicated by an arrow in the graphics area. You must properly define the direction for each hole using the Geometry list and the following options.

Cross Drill

After selecting Cross Drill, the following options become available.

Rotation Axis

This option must be set to the appropriate rotation axis of the part using one of the following options.

• Z Axis - is used when the rotation axis of the part is the Z-axis of the machine setup (machining origin).
  
  
• X Axis - is used when the rotation axis of the part is the X-axis of the machine setup (machining origin).
  
  
• Y Axis - is used when the rotation axis of the part is the Y-axis of the machine setup (machining origin).
  
  
• Pick Axis - allows you to define a custom rotation axis for the part by selecting geometry. After selecting Pick Axis, a selection box displays in the Rotation Axis group. Click in the box, and then select a line from the graphics area to define the rotation axis. The name of the selected entity displays in the box.
  

ID Drill

Select the check box when the drilling direction is outward or from the inside of the part to the outside.

Clear the check box when the drilling direction is inward or from the outside of the part to the inside.

Geometry

Selecting and Removing Geometry

The entities that you select in the graphics area display in the Geometry list. To remove geometry, right-click in the Geometry list to open a shortcut menu with the following options.

• Delete - Removes the currently selected items from the list.
  
  
• Delete All - Removes all geometry from the list.

You can also use the available buttons next to the Selected Geometry list:

Geometry Highlighting

You can click an entity name in the Geometry list to display that entity and direction in the graphics area using the system highlight color.

• Reverse - is used to reverse the drilling direction of the holes that are selected in the Geometry list.
  
  
• Reverse All - is used to reverse the drilling direction of all holes in the Geometry list.
  
  
• Delete - removes all currently selected holes from the holes list. This is helpful, for example, when selecting CAD features or using Select Whole Bodies and you want to remove individual holes from the selection, but not the entire selection.
  
  
• Delete - removes all currently selected holes from the holes list. This is helpful, for example, when selecting CAD features or using Select Whole Bodies and you want to remove individual holes from the selection, but not the entire selection.
  
  

Tip: You can also remove geometry selections by clicking entities in the graphics area, but note that this method clears the current selections in the Geometry list.

Selecting Multiple Entities in the Geometry List

The Geometry list allows for multiple selections using standard controls as follows.

• Click an entity name in the list to select it.
  
  
• Hold down theCtrl key and click an entity to add it to or remove it from the selection.
  
  
• After selecting one entity, hold the Shift key and click another entity to select all entities in between the first and second selections.