Drilling tab

You can use the Drilling tab of the Hole Feature Properties dialog to edit the drilling attributes for an Operation.

Drill operation:

Drill depth — Enter the absolute depth that the tool is driven into the stock, not including a point allowance. The Depth setting in the dimension attributes automatically includes a point allowance so use this attribute to override the point allowance. Alternatively use Drill depth adjust.This applies to Drill, Ream, Countersink, and Boring operations.

Drill depth adj. — Enter a positive or negative drill depth adjustment relative to the Hole feature's Depth dimension. Use this attribute instead of Drill depth if you prefer.

Note: If you enter both a Drill depth and a Drill depth adj. the adjustment is applied to the Drill depth value not the Depth dimension.

Spotdrill operation:

Spot drill depth — Enter the absolute depth that the spotdrill operation is driven into the stock.

Spot drill depth adj. — Enter the spot drill depth adjustment. You can enter a relative positive or negative spot drill depth adjustment to the Hole feature's Depth dimension instead of a Spot drill depth if you prefer.

Note: If you enter both a Spot Drill depth and a Spot Drill depth adj. the adjustment is applied to the Spot drill depth value not the Depth dimension.

Tap operation:

Max. tap spindle RPM — Enter the maximum speed, in RPM, for the tap operation.

Tap depth — This is an override for setting the depth of a tap operation.

By default, the system automatically sets a depth based on the thread depth and the geometry of the tap that is chosen. If it is a plug tap, five pitches are added to the requested tap depth. If it is a bottoming tap, three pitches are added to the requested tap depth.

If you enter a Tap depth value, no additional adjustment is made for the tap geometry, the Tap depth is passed straight to the NC code.

Tap plunge clearance — Enter the height above the feature where the tapping tool starts to feed into the feature.

Multi-axis drilling attributes

Multi-axis milling and drilling features have these attributes.

5-axis position menu — There is often an alternate orientation option for accessing a face. Select from:

• Standard — The default orientation.
• Alternate — The alternative orientation to the default.
• Use Post Preference — Uses the position (Positive or Negative) set in XBUILD in the Five Axis dialog for the Preferred orientation of the primary rotary axis option.
• Use Axis Limits — Allow FeatureCAM to select the orientation that best fits within the axis limits set in the MD file.

Index X coordinate — Optionally enter the absolute X coordinate to use for the index retract move.

Index Y coordinate — Optionally enter the absolute Y coordinate to use for the index retract move.

Index Z coordinate — Optionally enter the absolute Z coordinate to use for the index retract move.

If you do not enter a coordinate, the Z index clearance value is used for the index retract move. Z index clearance is a clearance distance above the stock bounding cylinder. This can result in a Z value for indexing that is outside the valid range for the machine. It can also result in less-efficient retract moves if the part is an irregular shape.

Orientation angle — Enter the initial C-axis position of the part in the machine at the start of the operation.