Bore is used for helical milling into a hole or a boss, with straight or tapered walls. Select any internal or external Face to create the path. The heights and depths are automatically derived from the selected Face.

Manufacture > Milling > 2D > Bore

Tool tab settings

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.

• 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)
• Ramp Spindle Speed - The rotational speed of the spindle when performing ramp movements
• Cutting Feedrate - Feedrate used in regular cutting moves. Expressed as Inches/Min (IPM) or MM/Min
• Feed per Tooth - The cutting feedrate expressed as the feed per tooth (FPT)
• Lead-In Feedrate - Feed used when leading in to a cutting move.
• Lead-Out Feedrate - Feed used when leading out from a cutting move
• Ramp Feedrate - Feed used when doing helical ramps into stock
• Plunge Feedrate - Feed used when plunging into stock
• Feed per Revolution - The plunge feedrate expressed as the feed per revolution

Geometry tab settings

Geometry

You can select Faces or a Diameter Range. Select any internal or external circular Face. Faces can be straight walled or tapered. Use Diameter Range to automatically include or exclude holes or bosses by specifying a minimum and maximum range.

Selection Mode

Select the geometry to machine by Faces or Diameter Range. Heights and depths are automatically derived from the selection.

Feature Type

Used with Diameter Range. Filters the hole selection.

Minimum and Maximum Diameter

Set the diameter range for the holes to include.

• Minimum - Holes equal to or greater than the specified value are included
• Maximum - Holes equal to or less than the specified value are included

Select Same Diameter

Used with Face selection. When enabled this includes all holes with the same diameter as the currently select 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.

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.

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.

Containment Boundary

Use this with Select Same Diameter 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.

Order

Specifies how the holes should be ordered for machining.

Reverse order

Enable to reverse the order of the sorted toolpath.

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:

• Setup WCS orientation - Uses the workpiece coordinate system (WCS) of the current setup for the tool orientation.
• Model orientation - Uses the coordinate system (WCS) of the current part for the tool orientation.
• Select Z axis/plane & X axis - Select a face or an edge to define the Z axis and another face or edge to define the X axis. Both the Z and X axes can be flipped 180 degrees.
• Select Z axis/plane & Y axis - Select a face or an edge to define the Z axis and another face or edge to define the Y axis. Both the Z and Y axes can be flipped 180 degrees.
• Select X & Y axes - Select a face or an edge to define the X axis and another face or edge to define the Y axis. Both the X and Y axes can be flipped 180 degrees.
• Select coordinate system - Sets a specific tool orientation for this operation from a defined user coordinate system in the model. This uses both the origin and orientation of the existing coordinate system. Use this if your model does not contain a suitable point & plane for your operation.

The Origin drop-down menu offers the following options for locating the triad origin:

• Setup WCS origin - Uses the workpiece coordinate system (WCS) origin of the current setup for the tool origin.
• Model origin - Uses the coordinate system (WCS) origin of the current part for the tool origin.
• Selected point - Select a vertex or an edge for the triad origin.
• Stock box point - Select a point on the stock bounding box for the triad origin.
• Model box point - Select a point on the model bounding box for 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

• Retract height: incremental offset from the Retract Height.
• Feed height: incremental offset from the Feed Height.
• Top height: incremental offset from the Top Height.
• Bottom height: incremental offset from the Bottom Height.
• Model top: incremental offset from the Model Top.
• Model bottom: incremental offset from the Model Bottom.
• Stock top: incremental offset from the Stock Top.
• Stock bottom: incremental offset from the Stock Bottom.
• Hole top: incremental offset from the Hole Top.
• Hole bottom: incremental offset from the Hole Bottom.
• Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
• Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

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

• Clearance height: incremental offset from the Clearance Height.
• Feed height: incremental offset from the Feed Height.
• Top height: incremental offset from the Top Height.
• Bottom height: incremental offset from the Bottom Height.
• Model top: incremental offset from the Model Top.
• Model bottom: incremental offset from the Model Bottom.
• Stock top: incremental offset from the Stock Top.
• Stock bottom: incremental offset from the Stock Bottom.
• Hole top: incremental offset from the Hole Top.
• Hole bottom: incremental offset from the Hole Bottom.
• Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
• Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

Retract Height Offset

Retract Height Offset is applied and is relative to the Retract 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

• Clearance height: incremental offset from the Clearance Height.
• Retract height: incremental offset from the Retract Height.
• Feed height: incremental offset from the Feed Height.
• Bottom height: incremental offset from the Bottom Height.
• Model top: incremental offset from the Model Top.
• Model bottom: incremental offset from the Model Bottom.
• Stock top: incremental offset from the Stock Top.
• Stock bottom: incremental offset from the Stock Bottom.
• Hole top: incremental offset from the Hole Top.
• Hole bottom: incremental offset from the Hole Bottom.
• Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
• Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

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

• Clearance height: incremental offset from the Clearance Height.
• Retract height: incremental offset from the Retract Height.
• Feed height: incremental offset from the Feed Height.
• Top height: incremental offset from the Top Height.
• Model top: incremental offset from the Model Top.
• Model bottom: incremental offset from the Model Bottom.
• Stock top: incremental offset from the Stock Top.
• Stock bottom: incremental offset from the Stock Bottom.
• Hole top: incremental offset from the Hole Top.
• Hole bottom: incremental offset from the Hole Bottom.
• Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
• Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

Bottom Offset

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

Passes tab settings

Tolerance

The tolerance used when linearizing geometry such as splines and ellipses. The tolerance is taken as the maximum chord distance.

CNC machine contouring motion is controlled using line G1 and arc G2 G3 commands. To accommodate this, Fusion approximates spline and surface toolpaths by linearizing them creating many short line segments to approximate the desired shape. How accurately the toolpath matches the desired shape depends largely on the number of lines used. More lines result in a toolpath that more closely approximates the nominal shape of the spline or surface.

Data Starving

It is tempting to always use very tight tolerances but there are trade-offs including longer toolpath calculation times, large G-code files, and very short line moves. The first two are not much of a problem because Fusion calculates very quickly and most modern controls have at least 1MB of RAM. However, short line moves, coupled with high feedrates, may result in a phenomenon known as data starving.

Data starving occurs when the control becomes so overwhelmed with data that it cannot keep up. CNC controls can only process a finite number of lines of code (blocks) per second. That can be as few as 40 blocks/second on older machines and 1,000 blocks/second or more on a newer machine like the Haas Automation control. Short line moves and high feedrates can force the processing rate beyond what the control can handle. When that happens, the machine must pause after each move and wait for the next servo command from the control.

Use Ramp Angle

Controls if the ramp feed depth is specified by a Pitch or by an Angle input value. Enable to specify the depth as an angular ramp depth.

Pitch

Specifies the Z distance to feed in per every 360° rotation. For straight walls this value is generally larger, than with tapered walls. A finer Pitch on a Tapered wall creates a smoother surface finish.

Angle

Specifies the maximum ramping angle of the helix during the bore cut.

Compensation Type

Specifies the compensation type.

• In computer - Tool compensation is calculated automatically by CAM, based on the selected tool diameter. The post-processed output contains the compensated path directly, instead of G41/G42 codes.
• In control - Tool compensation is not calculated, but rather G41/G42 codes are output to allow the operator to set the compensation amount and wear on the machine tool control.
• Wear - Works as if In computer was selected, but also outputs the G41/G42 codes. This lets the machine tool operator adjust for tool wear at the machine tool control by entering the difference in tool size as a negative number.
• Inverse wear - Identical to the Wear option, except that the wear adjustment is entered as a positive number.

Multiple Passes

Enable to enter a value for multiple depth cuts when Bore Milling.

Number of Stepovers

Enter the number of roughing steps. 2 Steps shown above.

Stepover

The maximum distance between finishing passes. (See the illustration shown above)

Finishing Passes

Enable to perform finishing passes using the side of the tool.

With Finishing passes

Without Finishing passes

Stepover

The maximum distance between finishing passes.

Repeat Passes

Enable to perform the final finishing pass twice to remove stock left due to tool deflection.

Direction

The Direction option lets you control if Fusion should try to maintain either Climb or Conventional milling.

Climb

Select Climb to machine all the passes in a single direction. When this method is used, Fusion attempts to use climb milling relative to the selected boundaries.

Left (climb milling) Climb Milling

Right (conventional milling) Conventional Milling

Use the Climb or Conventional Direction parameter to control Top to Bottom or Bottom to Top cut direction.

Stock to Leave

Positive Positive Stock to Leave - The amount of stock left after an operation to be removed by subsequent roughing or finishing operations. For roughing operations, the default is to leave a small amount of material.

None No Stock to Leave - Remove all excess material up to the selected geometry.

Negative Negative Stock to Leave - Removes material beyond the part surface or boundary. This technique is often used in Electrode Machining to allow for a spark gap, or to meet tolerance requirements of a part.

Negative Stock to Leave - Removes material beyond the part surface or boundary. This technique is often used in Electrode Machining to allow for a spark gap, or to meet tolerance requirements of a part.

Radial (wall) Stock to Leave

The Radial Stock to Leave parameter controls the amount of material to leave in the radial (perpendicular to the tool axis) direction, i.e. at the side of the tool.

Radial stock to leave

Radial and axial stock to leave

Specifying a positive radial stock to leave results in material being left on the vertical walls and steep areas of the part.

For surfaces that are not exactly vertical, Fusion interpolates between the axial (floor) and radial stock to leave values, so the stock left in the radial direction on these surfaces might be different from the specified value, depending on surface slope and the axial stock to leave value.

Changing the radial stock to leave automatically sets the axial stock to leave to the same amount, unless you manually enter the axial stock to leave.

For finishing operations, the default value is 0 mm / 0 in, i.e. no material is left.

For roughing operations, the default is to leave a small amount of material that can then be removed later by one or more finishing operations.

Negative stock to leave

When using a negative stock to leave, the machining operation removes more material from your stock than your model shape. This can be used to machine electrodes with a spark gap, where the size of the spark gap is equal to the negative stock to leave.

Both the radial and axial stock to leave can be negative numbers. However, the negative radial stock to leave must be less than the tool radius.

When using a ball or radius cutter with a negative radial stock to leave that is greater than the corner radius, the negative axial stock to leave must be less than or equal to the corner radius.

Linking tab settings

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).

• 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 moves instead of rapid movements (G0).

This parameter is usually set to avoid collisions at rapids on machines which perform "dog-leg" movements at rapid.

High Feedrate

The feedrate to use for rapids movements output as G1 instead of G0.

Safe Distance

Minimum distance between the tool and the part surfaces during retract moves. The distance is measured after stock to leave has been applied, so if a negative stock to leave is used, special care should be taken to ensure that safe distance is large enough to prevent any collisions.

Horizontal Lead-In Radius

Specifies the radius for horizontal lead-in moves.

Horizontal lead-in radius

Horizontal Lead-Out Radius

Specifies the radius for horizontal lead-out moves.

Horizontal lead-out radius

Linear Lead Length

Specifies the length of the linear leads.

Vertical Lead-In Radius

The radius of the vertical arc smoothing the entry move as it goes from the entry move to the toolpath itself.

Vertical lead-in radius

Vertical Lead-Out Radius

Specifies the radius of the vertical lead-out.

Vertical lead-out radius

Lead To Center

Specifies that the lead in/out movement should be into the center of the geometry.