Drill reference

Manufacture > Milling or Turning > Drill

Drilling is a common machining task for creating holes in the work piece. This function will usually trigger the CNC controls Canned Cycles. These cycles incorporate the common motion used for a specific hole machining task. There are usually Canned Cycles for basic drilling, deep hole drilling, counter boring, boring and tapping. The canned cycle output in the final code depends on the postprocessor and your machines capabilities.

These are the types of drilling motion that you can perform with this toolpath :

• Drilling - G81 style drilling with rapid out.
• Counterboring - G82 style drilling with dwell at bottom and rapid out.
• Chip breaking - Chip breaking with pecking and partial retracts between pecks.
• Deep drilling - Deep drilling with pecking and full retract between pecks.
• Guided deep drilling - gun drilling - Deep drilling that produces a round hole with a precision diameter. Useful for deep, straight holes in various materials.
• Tapping - Tapping (G84/G74). Synchronous spindle speed and feed.
• Tapping with chip breaking - Tapping with chip breaking.
• Break through - Allows for reduced feed and speed before breaking through a hole.
• Reaming - Reaming (G85 style) with feed out.
• Boring - Boring with dwell at bottom and feed out.
• Stop boring - Boring (G86 style) with spindle stop at the bottom and rapid out.
• Fine boring - Fine boring with shift away from the hole side.
• Back-boring - Boring from the back.
• Circular pocket milling - Circular pocket milling.
• Bore milling - Bore milling.
• Thread milling - Thread milling.
• Probe - Used to measure a feature on the part with a probe tool, or use macros from the machine to define the WCS. Needs special handling in the post processors depending on the machine.

Need more information on these canned cycles?

The input geometry for these cycles can be selected directly from the features of part geometry, and consistent with other 2D operations, input geometry can also be selected from a sketch, (for example: center points of arcs).

When working with solid models, the easiest way to use Drilling is to select the cylindrical faces of the holes. This automatically sets the correct stock height and depth for each hole. Drilling will recognize holes with different starting heights and depths, to create a single drill operation. Notice that when from cylindrical faces, the Select Same Diameter option is available. This allows easy - automatic - selection of any similar holes.

For more information, watch the Spot drilling holes video.

Tool tab settings

Tool

Press Select to access the tool library.

Feed & Speed

Spindle and Feedrate cutting parameters.

• Preset - Populates custom tool's cutting data.
• Spindle Speed - The rotational speed of the spindle expressed in Rotations Per Minute (RPM).
• Surface Speed - The speed which the material moves past the cutting edge of the tool (SFM or m/min).
• Use Feed per Revolution - Changes input of the feedrate to units per spindle's revolution instead of distance over time.
• Plunge Feedrate - The drilling feedrate when plunging into stock.
• Plunge Feed per Revolution - The plunge feedrate expressed as the feed per revolution.
• Retract Feedrate - Feed used when retracting, but not using rapid moves (G0).
• Retract Feed per Revolution - The retract feedrate expressed as the feed per revolution.
• Coolant - Select the type of coolant used with the machine tool. Not all types will work with all machine postprocessors.

Flute, Shaft & Holder

Specifies how the flute, shaft and holder of the tool is used to avoid collisions with the workpiece.

• Shaft and Holder Mode - Specifies how to handle a collision between the shaft or holder and the part when performing cutting moves.

  • Trimmed - When a collision is detected on a cutting move, the safe part of the move is retained and the colliding part is trimmed away. Pairs well with Remaining holes from operation in Selection Mode on the Geometry tab. An initial operation with Trimmed selected can use a shorter, more stable tool to remove the majority of material in the holes. A following operation can then select the remaining holes that need finishing from the first operation, and drill them with a longer tool that can reach the bottom of the holes. Any number of operations can be chained together to machine a set of holes with increasingly longer tools.

    Note: When Trimmed is selected, some cycle types are not available, including Break through, Guided deep drilling - gun drilling, Tapping, Reaming - feed out, and Back-boring.

  • Detect tool length - The tool is automatically extended further out of the holder to maintain the specified clearances. A message indicating how far the tool is extended appears in the toolpath log.

  • Fail on collision - Aborts toolpath calculation when a collision is detected.

  • Skip colliding holes - Skips any holes where collisions are detected. The tool moves onto the next available hole that is safe to cut.

• Use Shaft and Holder - Enable to include the shaft and holder of the selected tool in the toolpath calculation to avoid collisions. When selected, specify Shaft Clearance and Holder Clearance to set the minimum safe distance from the workpiece.

• Shaft Clearance - The tool shaft always stays this distance from the workpiece.

• Holder Clearance - The tool holder always stays this distance from the workpiece.

• Use Flute - Checks for gouges using the tool's flute length during cutting moves only. When using Points in Selection Mode, gouges are expected, so this option is not applicable.

• Check Machine Spindle - Specifies that the spindle of the machine used by this setup is included in the toolpath calculation to check for collisions.

• Check Machine Table - Specifies that the table of the machine used by this setup is included in the toolpath calculation to check for collisions.

Multi-Axis tab settings

Machining Type

• 3-axis - Standard drilling with a fixed Z-axis. Use this for vertical holes aligned with the Z-axis.

• Polar - Uses polar linking for drilling operations while keeping cycle output for cutting moves. This can help you stay within machining limits when necessary. Only holes aligned with the same axis are machinable in this mode. You can select holes on a planar face, often the end of a cylinder. For more information, see Polar machining.

• 4-axis - Define a rotary axis for your machining setup. By default, holes are drilled perpendicular to this axis. Use this for holes that are not aligned with the Z-axis, such as angled holes or holes on a sloped surface:

  • Specify whether hole axes must intersect the rotary axis, in cases like holes on a cylinder.

  • Allow hole axes to shift in the perpendicular plane, in cases like holes on a cuboid.

  • Set a tilt angle to tilt holes away from the perpendicular plane.

    For more information, see 4-axis machining.

• 5-axis - Machine holes using full 5-axis movements. Use this for complex hole geometries that need the tool to tilt to reach certain areas. You can define axis limits and set minimum and maximum tilt angles relative to the tool axis. For more information, see 5-axis machining.

Tool orientation

The tool orientation defines the cutting plane on a part. By default, the Z axis of the work coordinate system (WCS) that is defined in a setup sets the orientation of the tool. You can override the tool orientation set by the WCS using the Tool Orientation group of settings.

For more information, check the Set a tool orientation page.

Geometry tab settings

Geometry

Allows you to select drilling locations by model face, hole edge, sketch point, sketch circle, or a diameter size range. You can also inherit locations from a previous operation to finish holes that could not be completed in the original operation.

Selection Mode

Specifies which type of selections will be used for finding the drilling locations.

• Faces - Model-based feature selection for cylinders or hole chamfers. Provides starting height and hole depth. Preferred method because it maintains associativity to the model feature. Select holes using Hole Faces.

• Points - Geometry-based selection for hole edges or sketch geometry. Returns only the XY location and Z starting height of the hole. Select holes using Hole Points.

• Diameter range - Automatic selection based on a minimum and maximum hole size. Specify Minimum Diameter and Maximum Diameter to include or exclude hole sizes without selecting features on the model. Example: Select all .250–.2501 in. holes for drilling and all .2505–.2506 in. holes for reaming.

• Remaining holes from operation - Operation-based selection for fallback drilling. Selects holes left unmachined or partially machined by a specified reference operation and applies its key settings, such as Heights and Cycle Parameters, to ensure consistency. Select a preceding operation using Operation. Use this option to create secondary operations that typically use longer tools to reach areas where the primary operation encountered collisions.

  Note: The reference operation must have Flute, Shaft & Holder collision checking enabled. To pass entire holes to a follow-up operation when a collision is detected, set Shaft and Holder Mode to Fail on collision or Skip colliding holes on the primary operation. To machine partial depths and finish with longer tools, set Shaft and Holder Mode to Trimmed on the primary operation.

Faces selection - Cylinder	Faces selection - Chamfer
Points selection - Hole Edge	Points selection - Sketch Point	Points selection - Sketch Circle

Select Same Diameter

Selects all holes with the same diameter as the currently selected feature.

A single selection will find all matching holes. Using this option is associative to the model. If additional holes with the same diameter are added later, regenerating the operation automatically includes the added holes in the drilling cycle.

Example: If you activate this option, select a single 6mm hole and a single 12mm hole, every 6mm and 12mm hole on the part will automatically be selected.

Check for Occlusions

Deselects any holes of the same diameter that cannot be drilled because of the current tool orientation.

For example, if a hole is on the underside of a part and the drill cannot reach it, the hole is not drilled.

Deselected	Selected

Containment Boundary

Use this with Select Same Diameter and Diameter Range to include similar items inside the containment areas. Select any Edge or Sketch boundary to contain the drilling locations. Use multiple boundaries or nested boundaries, to include or exclude groups of holes. The toolpath will be inside the selected boundary unless the boundaries are nested. You can nest several boundaries inside each other.

In the examples below, the selected boundaries are shown in blue.

	1) Sketch Boundaries 2) Holes inside are included 3) Nested Boundaries 4) Inside areas are excluded	5) Sketch Boundaries (2) 6) Selecting the rim area only 7) Sketch Boundaries (3) 8) Excluding the rim area

Auto-Merge Hole Segments

Check to merge multiple hole segments. When enable all hole segments are included to determine the starting height for drilling. Use this option when the selected drill hole has a counter bore. This will force the starting height to be at the top of the counter bored hole, rather than the top of the drilled hole.

Example: If a hole was Spot Drilled or Counter Bored first, you may want to start drilling from a clearance above that machined area. Enabling Auto-Merge will start the drilling from above the highest hole segment.

	Left Side Hole: Auto-Merge Disabled Right Side Hole: Auto-Merge Enabled Blue line indicates the starting height for drilling

Order by Depth

Changes the order from the highest to lowest, or lowest to highest. Unchecked, the order will start with the holes at the highest Z level and progressively move down. Check to reverse the order.

Deselected First hole is at the highest Z	Selected First hole is at the lowest Z

Order

Specifies how the holes should be ordered for machining.

	1) Order selected 2) Optimized order 3) Inside to Outside 4) Order by X motion 5) Order by Y motoion

Reverse Order

Select to change the order of the sorted toolpath.

Deselected	Selected

Reset Directions

Reverts all manually fixed through hole directions back to default. Default directions may change automatically to avoid collisions.

Fixed directions	Default directions

Surface Manager

Lets you specify surfaces to machine, avoid, ignore, or mark as fixtures to avoid during toolpath calculation. For more information, check Surface Manager page.

Heights tab settings

For Clearance Geometry, see Clearance geometry.

For machining heights, see Setting machining heights and:

• Clearance height
• Retract height
• Feed height
• Top height
• Bottom height

Drill Tip Through Bottom

When Enabled the tool tip will drill past the bottom of the hole. It positions the lip of the drill to the full diameter at the bottom of the hole. It also allows the tool to drill completely through the bottom, or past the bottom using the Break-Through Depth.

Left Side Hole: Depth is to the Tip (unchecked) Right Side Hole: Depth is to the Lip (checked)

Cycle tab settings

Cycle Type

The Cycle type is the type of drilling cycle. Fusion provides a number of predefined (canned) drilling cycles.

Selecting a drill cycle determines which parameters can be specified for the drilling operation.

• Drilling - rapid out - Feed in to the programmed depth and rapid out. Used for Center Drilling, Spot Drilling and holes with depths of less than three times the tool diameter.
• Counterboring - dwell and rapid out - Feed in to the programmed depth, dwell for a specified time and rapid out. Used to create a flat bottom on shallow clearance for screws. The dwell improves the finish on the floor of the hole.
• Chip breaking - partial retract - For holes with depths of more than three or four times the tool diameter tool. Uses multiple pecks that periodically retracting the tool to break the chips and/or allow coolant to enter the hole. This is also known as Peck drilling.
• Deep drilling - full retract - Similar to Chip breaking, but retracts the tool completely out of the hole to clear chips and/or flood the hole with coolant. This is also known as Peck drilling.
• Break through - Allows for reduced feed and speed before breaking through a hole.
• Guided deep drilling - gun drilling - A standard gun drill has a single effective cutting edge. This unique head geometry is different from a conventional twist drill. While drilling, guide pads burnish the hole allowing the hole to maintain straightness. The result of this activity is a very round hole with a precision diameter that can also produce deep, straight holes in a variety of materials.
• Tapping - Tapping is a process that cuts threads into a hole, to accept screws. Taps right or left threads in a round hole with a multi-point tool that looks similar to a screw.
• Left tapping - Creates a threaded hole for left handed screws. The tap rotates counterclockwise as it enters the hole and reversed to exit the hole.
• Right tapping - Creates a threaded hole for right handed screws. The tap rotates clockwise as it enters the hole and reversed to exit the hole.
• Tapping with chip breaking - Creates a threaded hole by feeding in and out multiple times, going deeper each time, until it reaches the final depth.
• Reaming - feed out - Feeds in and immediately feeds out after reaching the final depth. This is a precision hole finishing operation.
• Boring - dwell and feed out - Similar to Reaming, but includes a dwell at the bottom depth.
• Stop boring - stop and rapid out - Feeds in to the depth, stops the spindle rotation and rapids out. This does drag the boring insert along the wall during the retract.
• Fine boring - shift Similar to Stop Boring, except that it will orient the tip of the insert and move it away from the wall of the bore before performing the retract move.
• Back-boring - moves to a depth inside the hole and stops, while a reverse counterboring tool is attached. The spindle then starts and the tool feeds up, to counter bore the back side of the part.
• Circular pocket milling - This can be used to initiate a custom canned cycle on the control for circular pocketing.
• Bore milling - This can be used to initiate a custom canned cycle on the control for helical bor milling.
• Thread milling - This can be used to initiate a custom canned cycle on the control for thread milling.
• Custom - Used to measure a feature on the part with a probe tool, or use macros from the machine to define the WCS. Needs special handling in the post processors depending on the machine. See the more advanced Probing function, under the Setup pull down.

Additional parameters appear on the Cycle tab depending on the cycle type you select. For cycle motion diagrams and parameter descriptions, see Drilling Cycles reference.

Trimmed Holes

On a follow-up Drill operation—not the primary operation where Trimmed is set—the Trimmed Holes group appears on the Cycle tab when Selection Mode is Remaining holes from operation and the reference operation used Trimmed in Shaft and Holder Mode.

• Starting Depth Offset - Specifies the starting depth of the drilling cycle inside the hole, measured as an offset from the remaining uncut material of the partially machined hole.
• Positioning Feedrate - Sets the speed of the tool as it moves from the Top Height to the Starting Depth Offset during air cutting.
• Positioning Spindle Speed - Sets the rotational speed of the spindle as the tool moves from the Top Height to the Starting Depth Offset during air cutting.

Linking tab settings

Specify how toolpath passes should be linked.

Linking

• Ignore Gouges - Avoids checking for gouges when performing linking moves to help speed up initial toolpath calculation, particularly on larger models. Gouge checking occurs between the tool's flutes and the model.

  Important: Use this option to speed up initial programming of the operation. After finalizing the operation, recalculate the operation once more with this option deselected to help detect any possible gouges.

• Retraction Policy - Specifies how to handle a possible collision when performing link moves.

  • Avoid collisions - Avoids gouges between the cutting portion of the tool and the model. To avoid collisions between the shaft or holder and the part, on the Tool tab, enable Flute, Shaft & Holder and specify Shaft Clearance and Holder Clearance.
  • Preserve cycles - Does not adjust the retract height when encountering a possible collision. Instead, a warning appears in the toolpath log to inform you of the collision.

• High Feedrate Mode - Specifies when rapid movements should be output as true rapids (G0) and when they should be output as high feedrate movements (G1). This parameter is usually set to avoid collisions at rapids on machines which perform "dogleg" movements at rapid.

  • Preserve rapid movement - All rapid movements are preserved.
  • Preserve axial and radial rapid movement - Rapid movements moving only horizontally (radial) or vertically (axial) are output as true rapids.
  • Preserve axial rapid movement - Only rapid movements moving vertically.
  • Preserve radial rapid movement - Only rapid movements moving horizontally.
  • Preserve single axis rapid movement - Only rapid movements moving in one axis (X, Y, or Z).
  • Always use high feed - Outputs rapid movements as high feed moves (G01) instead of rapid movements (G0).

• Safe Distance - Sets the minimum distance between the tool and the part's surfaces during retract moves. Within this distance, the tool retracts with a direct move, instead of a rapid move. The distance is measured after stock to leave is applied. If a negative stock to leave is used, make sure that Safe Distance is large enough to prevent any collisions.