Drill reference

drilled part example

Manufacture > Milling or Turning > Drill drill icon

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 you can perform with this toolpath :

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.

Interested in a structured lesson on Drilling? Drilling Lesson

tool tab icon Tool tab settings

drill dialog tool tab

Coolant

Select the type of coolant used with the machine tool. Not all types will work with all machine postprocessors.

Feed & Speed

Spindle and Feedrate cutting parameters.

geometry tab icon Geometry tab settings

     

Watch this short animation for an overview of the hole selection filters.

drill hole selection options animation

Hole Mode

Specifies which type of selections will be used for finding the drilling locations. Selecting Faces provides additional information like the starting height and hole depth. Selected Points will only return the XY location and Z starting height of the hole. Selected Faces is the preferred method for picking drilling locations because it maintains associativity to the Model Feature and will update the drilling operation if the model changes.

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

Hole Faces

Contains the number of faces selected for drilling. This is for Model based feature selection. Use the X to clear all the currently selected items.

Hole Points

Contains the number of points or edge curves selected for drilling. This is for Geometry based hole selection. Use the X to clear all the currently selected items.

Diameter Range

Opens a parameter set for creating a minimum and maximum range selection. Eliminates the need to physically select features from the model. The system will evaluate the model based on the Minimum and Maximum Diameter values specified. Use this range to include or exclude hole sizes. This is useful If the part is modeled with sizes that represent different machining processes.

Example: Select all .250 - .2501 diameter holes for drilling and all .2505 - .2506 diameter holes for reaming.

Tip: To Spot drill all the holes and create a chamfer - Select a Range for the holes to include. On the Heights tab, set the Bottom Height from Chamfer Width and set the desired Chamfer Width value. The depth will be based on the hole diameter + chamfer width.

Select Same Diameter

Check to select all holes with the same diameter as the currently select feature.

select same diameter example

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.

Only Same Hole Depth

Check to select all the holes that share the same top to bottom distance as the currently select feature.

Example: You can use this as a way to distinguish between 6mm tapped holes and 6mm drilled holes of different depths.

   
Short Depth 6mm holes selected - ISO view Short Depth 6mm holes selected - Front view
Short Depth 6mm holes selected - ISO view Short Depth 6mm holes selected - Front view
Long Depth 6mm holes selected - ISO view Long Depth 6mm holes selected - Front view
Long Depth 6mm holes selected - ISO view Long Depth 6mm holes selected - Front view

Only Same Z Top Height

Check to select all the holes that share the same Z top height as the currently select feature.

You can use this as a way to limit machining to one Z level. The red arrow below indicates the selected feature.

   
All Short Depth Holes, at the Mid Level Height All Short Depth Holes, at the Mid Level Height

All Long Depth Holes, at the Lower Level Height.
All Short Depth Holes, at the Mid Level Height Short Depth 6mm holes selected - Front view

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.

   
Check for occlusions deselected check for occlusions selected
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.

     
Containment Boundary animation 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.

   
Merge hole segments 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.

   
Disabled.

First hole is at the highest Z		 Enabled.

First hole is at the lowest Z
Order Top Down Order Bottom Up

Order

Specifies how the holes should be ordered for machining.

   
Optimize hole selection animation 1) Order selected

2) Optimized order

3) Inside to Outside

4) Order by X motion

5) Order by Y motoion

Reverse order

Check to change the order of the sorted toolpath.

   
Disabled Enabled
Order inside out Order outside in

Tool Orientation

Allows you to redefine the machining plane, if it's different than the Tool Plane in the Setup and change the Work Coordinate System Origin (WCS - XYZ zero). The Tool Orientation sets the working XY machining plane and allows you to tilt the spindle axis (Z). This can be used for 4th axis indexing and 5 axis positioning. Also referred to as 3+2 axis position.

The Orientation drop-down menu provides the following options to set the orientation of the X, Y, and Z triad axes:

The Origin drop-down menu allows you to shift the Work Coordinate System Origin (WCS - XYZ zero). It offers the following options for locating the origin:

heights tab icon Heights tab settings

drill dialog heights tab

Clearance Height

The Clearance height is the first height the tool rapids to on its way to the start of the tool path.

clearance height diagram

Clearance Height

Clearance Height Offset

The Clearance Height Offset is applied and is relative to the Clearance height selection in the above drop-down list.

Retract Height

Retract height sets the height that the tool moves up to before the next cutting pass. Retract height should be set above the Feed height and Top. Retract height is used together with the subsequent offset to establish the height.

retract height diagram

Retract Height

Retract Height Offset

Retract Height Offset is applied and is relative to the Retract height selection in the above drop-down list.

Feed Height

Feed height sets the height that the tool rapids to before changing to the feed/plunge rate to enter the part. Feed height should be set above the Top. A drilling operation uses this height as the initial feed height and the retract peck height. Feed height is used together with the subsequent offset to establish the height.

feed height diagram

Feed Height

Feed Height Offset

Feed Height Offset is applied and is relative to the Feed height selection in the above drop-down list.

Top Height

Top height sets the height that describes the top of the cut. Top height should be set above the Bottom. Top height is used together with the subsequent offset to establish the height.

top height diagram

Top Height

Top Offset

Top Offset is applied and is relative to the Top height selection in the above drop-down list.

Bottom Height

Bottom height determines the final machining height/depth and the lowest depth that the tool descends into the stock. Bottom height needs to be set below the Top. Bottom height is used together with the subsequent offset to establish the height.

bottom height diagram Bottom Height

Bottom Offset

Bottom Offset is applied and is relative to the Bottom height selection in the above drop-down list.

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)

Break-Through Depth

Specifies how far the lip of the tool drills past the bottom of the hole, to ensure a clean cut through the part.

 

Left Side Hole: Break Through 0.0 in.

Right Side Hole: Break Through 0.06 in.
Important: Break-through might cause the tool to cut into the fixture or material below the part.

cycle tab icon Cycle tab settings

drill dialog cycle tab

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.

Pecking Depth

Sets the depth for the first peck move, which plunges in and out of the material to clear and break chips.

Pecking Depth Reduction

The amount by which the pecking depth is reduced per peck.

Minimum Pecking Depth

The minimum allowed pecking depth.

Accumulated Pecking Depth

Specifies the pecking depth which forces full retract.

Chip Break Distance

With a chip breaking operation, the drill withdraws a specified distance after advancing into the hole to prevent the binding of chips.

Dwell Before Retract

Enables dwelling before pecking retracts to thin out chips. This can increase tool lift significantly depending on the material being machined.

Dwelling Period

The Dwelling period is the dwelling time in seconds. Specifying a dwell time halts all axis movement for a specified time while the spindle continues revolving at the specified rpm. This can be used to ensure that chips are cleared before retracting from a hole, and will typically improve the finish of a hole.

Typically a dwelling time between 1/4 second and 1 second is sufficient. As an example, specify 0.25 or 1/4 in this field to dwell for 1/4 second.

When post processing a drill cycle, the dwell time is specified as one of the drill cycle parameters (typically P), and in most cases it is output in milliseconds (ms).

dwelling period diagram

250ms dwell time in G82

When posting using expanded cycles, the dwell time is output as a regular dwell command (G4).

To calculate the minimum dwell time that will ensure at least one complete revolution, use a value of 60 divided by the spindle speed. As an example, at 350 RPM the minimum dwell time should be 60 / 350 = 0.171s (which could be rounded to 0.2s).

Note: If an operator is running the program with a speed override, then the spindle speed is slower, but the dwell time is constant. To ensure one complete revolution when using a speed override of 50%, for example, the dwell time must be doubled.
Parent page: Drill strategy