About Drill



Access:

Ribbon: CAM tab Drilling panel Drill

A Drill operation provides access to a whole range of drilling, tapping and hole making operations. These include:

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 the drill feature is to select the cylindrical faces of the holes to drill directly. This automatically sets the correct stock height and depth for each hole, and allows having holes in different planes and different depths in a single drill feature. Observe also that when drilling from cylindrical faces, the Select same diameter option is available, and allows easy - and automatic - selection of many similar holes.

Tool tab settings



Coolant:

The type of coolant used with the tool.

Spindle speed:

The rotational speed of the spindle.

Surface speed:

The spindle speed expressed as the speed of the tool on the surface.

Plunge feedrate:

Feed used when plunging into stock.

Feed per revolution:

The plunge feedrate expressed as the feed per revolution.

Retract feedrate:

Feed used when retracting and not using rapid (G0) moves.

Geometry tab settings



Select same diameter

Check this to automatically select all holes with the same diameter as the hole currently selected in the selection box.

Example: To drill a single 6 mm / 1/4" hole and all 12 mm / 1/2" holes, first select the 6 mm / 1/4" hole, then select one of the 12 mm / 1/2" holes, and then check the Select same diameter option.

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.

Auto-merge hole segments

When drilling a hole with multiple segments, enable to have neighboring segments included automatically.

Order by depth

Specifies that the holes must be ordered by either increasing or decreasing Z-level.

Optimize order

Specifies that the holes should be ordered such that the machining distance is minimized.

Order inside-out

Enable to reorder holes from the default order to an order which machines inner holes first and then outer holes.

Tool Orientation

Specifies how the tool orientation is determined using a combination of triad orientation and origin options.

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 offers the following options for locating the triad origin:

Heights tab settings

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

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

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

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

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

Bottom offset:

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

Drill tip through bottom

Enable to make the tool tip drill completely through the bottom.

Break-through depth:

Specifies how far the tool drills past the bottom of the hole to ensure through-cutting.

Caution: Break-through might cause the tool to cut into the fixture or material below the part.

Cycle tab settings



Cycle type:

The Cycle type is the type of drilling cycle. Inventor HSM 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).



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.
Topics in this section
Parent topic: Drill Reference