RabbitCAM X Support

Smart Drilling Overview

Smart Drilling calculates a final tool-tip depth separately for each assigned hole position. It finds the top of the remaining material, then evaluates how far the cutting portion of the tool can descend within the modeled geometry and the operation's limits.

The result is limited by Bottom Level, the tool's cutting length, and contact with the Part or protected Work Holding. Different holes in one operation can finish at different Z values, and positions with no available downward cut can be skipped.

Three strategies are available: Simple, Chip Removing, and Chip Breaking. They use the same calculated depths and differ in how the drilling moves reach them.

For manually specified Start/End Levels, see Drilling. For a fixed relative tip depth below each local material surface, see Spot Drilling.

Creating the Operation and Selecting a Tool

1. Prepare the Part, Stock, Workpiece Coordinate System, and any modeled Work Holding.
2. Open Machining > New Operation and select Smart Drilling under Hole Machining.
3. Review the operation name. Choose a suitable Drill, Center Drill, or End Mill with the ... tool-selection button, then click Create.
4. Select the new operation, assign its positions in Job Assignment, and open Strategy.
5. Choose the drilling strategy and set Bottom Level, Approach Clearance, Safe Level, and the cutting parameters.

Smart Drilling supports Drill, Center Drill, and End Mill tools. Review the diameter, cutting profile, cutting length, and stickout: these values affect whether the tool fits and how deep it can go.

With an End Mill, Smart Drilling still makes axial drilling moves at each center; it does not generate a helical entry or clear the whole boundary as a pocket. The flat cutting profile is used when checking the available depth.

Use a 3D Part with surface geometry for the depth calculation. Standalone curves or a curve-only DXF do not provide the Part surfaces needed by this operation.

Assigning Hole Positions

1. Open Job Assignment and choose Pick > Boundary.
2. Select the closed boundaries defining the intended hole positions.
3. Choose Finish Boundary Selection and review the Drilling References list.

A Boundary produces one position at the area centroid of its XY projection. It must be closed, continuous, and enclose a valid projected area. Check the center of an irregular boundary before machining.

Compatible Circle and Boundary references can also be copied and pasted from other drilling operations. A Circle reference must resolve to a full horizontal circle. The current Smart Drilling Pick menu offers Boundary selection.

The reference supplies the XY center. Its CAD Z does not set the material surface or final depth, and its size does not automatically change the assigned tool diameter. References with the same XY center are combined into one position, retaining the first occurrence.

How the Depth Is Calculated

For each unique position, Smart Drilling performs the following calculation:

1. Find the top of the remaining material before this operation at that XY location.
2. Check the tool's cutting profile against the modeled Part and Work Holding at the local starting surface.
3. Evaluate progressively lower positions, stopping at the first detected interference or at the limit imposed by Bottom Level and cutting length.
4. If interference is detected during descent, move the calculated endpoint upward until the cutting profile has a position accepted by the geometry check.

The Part represents the finished geometry to retain. Modeled holes and cavities provide space for the tool to descend; their walls and floors can limit that descent. Selecting a Boundary identifies a center but does not create a new opening in an otherwise solid Part.

Work Holding checks include the configured safety clearances. The depth check uses the cutting portion of the tool; it does not check the shank or holder, or provide automatic clearance for all rapid transfers.

The endpoint is a calculated tool-tip position. Geometric approximation and collision tolerances can leave it slightly above a modeled contact surface. Review the resulting depth and required hole dimensions in Simulation.

If the tool is blocked at the starting surface, that position is skipped. A position whose local surface is already at or below Bottom Level also receives no downward drilling move. Missing remaining material at a selected center is reported as an error.

Setting Bottom Level

Bottom Level is the lowest permitted tool-tip Z in work coordinates. It applies to every assigned position, but a hole can finish above it because of geometry or cutting length.

Enter the required Z directly or use the pick button beside Bottom Level. Picking a surface uses its lowest Z, converted to work coordinates.

Where the descent is unobstructed, the lower limit is:

Final tip Z = max(Bottom Level, Local material top Z − Cutting Length)

This formula applies when Bottom Level is below the local surface. A more negative Bottom Level permits a deeper search, but cannot extend the tool's cutting length or force it through protected geometry.

Smart Drilling has no manual Start Level, relative Hole Depth, or Drill Tip/Full Diameter selector. The local starting surface is calculated from the remaining material, and Bottom Level limits the tip. With a pointed drill, the full-diameter portion of a hole ends above the tip.

Approach Clearance and Safe Level

Approach Clearance is the distance above the local material surface where rapid descent ends and drilling feed begins. The default is 2 mm; zero or positive values are accepted.

Approach Z = Local remaining-material top Z + Approach Clearance

For example, a local surface at work Z-3 mm with 2 mm clearance gives an approach point at Z-1 mm.

Safe Level is the work-coordinate Z used for travel between hole positions and for the final retract from each hole. It is a coordinate, not an additional distance above the local surface.

Set Safe Level at or above every approach point that will be machined, and high enough to clear the setup during travel. The current generator uses the entered value; it does not raise it automatically. If an approach point is higher than Safe Level, generation stops and reports the required minimum for that position.

With a local surface at Z0 and Approach Clearance of 2 mm, the approach is Z+2 mm, so Safe Level must be at least Z+2 mm. The actual travel height may need to be higher to clear part features and fixtures.

Choosing the Drilling Strategy

• Simple feeds continuously from the local approach point to the calculated final depth, then retracts to Safe Level.
• Chip Removing drills in pecks. Between intermediate pecks, it retracts to the local approach point, then returns rapidly to a position above the previous depth before feeding again.
• Chip Breaking drills in pecks with a short rapid retract between intermediate pecks, followed by feed to the next depth.

The Cycle fields change with the strategy. Simple has no peck settings. Chip Removing shows Peck Depth and Reentry Clearance. Chip Breaking shows Peck Depth and Chip Break Retract.

The selected strategy changes the motion sequence, while the geometric calculation supplies the endpoint for each hole.

Peck Depth and Retraction Settings

Peck Depth is the maximum new depth cut in each increment, measured from the local material surface. It must be positive. A shorter final increment is used when needed to reach the calculated endpoint.

For a local surface at Z0, a calculated endpoint of Z-7 mm, and Peck Depth = 2 mm, the pecks finish at Z-2, Z-4, Z-6, and Z-7 mm. Approach Clearance does not add another cutting-depth increment.

For Chip Removing, Reentry Clearance determines how far above the previous peck depth the rapid return stops. The position is capped at the local approach height. For example, after reaching Z-4 mm, a 0.5 mm reentry clearance stops the rapid return at Z-3.5 mm before the next feed.

For Chip Breaking, Chip Break Retract sets the short upward rapid move after each intermediate peck. Its endpoint is also capped at the local approach height. The following feed descends from that retracted position to the next peck depth.

Reentry Clearance and Chip Break Retract must be positive. The defaults are Peck Depth = 2 mm, Reentry Clearance = 0.5 mm, and Chip Break Retract = 0.5 mm. After the final peck, both strategies retract to Safe Level.

RPM and Drilling Feed Rate

• RPM sets spindle speed in revolutions per minute.
• Drilling Feed Rate sets the axial cutting feed in mm/min, including each peck.

Both values must be positive. Approach, reentry, and retract moves use rapid motion. Choose spindle speed and feed for the actual tool and material, and review them after changing tools or strategies.

Example: Different Limits for Different Holes

Assume Bottom Level = -12 mm and a tool with 8 mm cutting length. For positions where the cutting profile can descend without interference, the limits are:

A wall, floor, or protected Work Holding region can make another position finish higher. If the cutting profile is blocked at the local starting surface, that position is skipped.

These are level-calculation examples, not cutting recommendations. Changing the preceding operations can change the local surface heights and therefore the calculated results.

Hole Order and Toolpath Verification

Smart Drilling retains Job Assignment order for the unique centers. Skipped positions produce no drilling moves.

For each machined hole, the tool moves vertically to Safe Level, travels in XY to the center, descends rapidly to the local approach point, executes the selected cycle, and retracts vertically to Safe Level. Transfers between holes use the entered Safe Level.

1. Confirm the modeled holes or cavities, assigned centers, tool geometry, and operation order.
2. Set Bottom Level, Approach Clearance, Safe Level, and the selected cycle's parameters.
3. Click Run & Link and select Smart Drilling to inspect the generated paths.
4. Open Simulation. Check which positions are machined, their final tip depths, the peck sequence, and all approaches, transfers, and retracts.
5. Recalculate after changes to the Part, references, tool, Stock, Work Zero, Work Holding, preceding operations, or strategy settings.
6. Save with Ctrl+S and use Post Process when the setup is ready.

A successful calculation does not mean every selected position reached Bottom Level. Compare the machined positions with the assigned references and check individual depths, including any positions with no toolpath.

Common Problems

• Invalid tool: select a Drill, Center Drill, or End Mill. Check the cutting profile, positive cutting length, and adequate stickout.
• Missing machining geometry: use a Part containing valid 3D surfaces; standalone reference curves are insufficient for the depth search.
• No remaining material at World X/Y: review the assigned center, Stock position, and material left by earlier operations. These error coordinates are model/world coordinates.
• Safe Level is too low: increase it to cover all required approach heights and the travel clearance, then recalculate.
• A hole is shallower than expected: review Bottom Level, cutting length, tool diameter and cutting profile, Part walls or floors, and Work Holding safety clearances.
• A selected position has no drilling moves: check for duplicate XY centers, an initial tool/geometry collision, or a local surface already at or below Bottom Level. All positions can be skipped if none permits a downward cut.
• A reference is rejected: use a closed, continuous Boundary with a valid projected area, or a compatible full horizontal Circle reference.
• Invalid cycle values: use positive Peck Depth and the positive retraction setting required by the selected strategy.

For related setup, see Setting the Workpiece Coordinate System and Setting Up Work Holding. For NC export, see JavaScript Post Processors.