The Face toolpath strategy is designed for quick removal of the raw stock from the top surface of the part. It generally prepares the part for further machining. It's used for clearing flat areas.

Manufacture > Milling > 2D > Face

Interested in a structured lesson on 2D Face?

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

Stock Contours

The Face toolpath assumes you want to machine the top of the stock to a depth of Z0. Generally No Selections Is Required For The Face Toolpath. The system will automatically face the size and shape of the Stock defined in the job Setup parameters. If you want to Face a specific area, use the Stock Selections option shown below. The stock area to machine is shown in Yellow.

No selection is required to machine the default Stock.

Stock Selections

You can select any size or shape area to apply the Face toolpath. This area can be an Edge selection or a Sketch selection. No selection is needed if you want to face the area defined in the job Setup, Stock definition. The stock area to machine is shown in Yellow.

Default stock area shown in yellow.

Edge selection of Facing boundary.

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.
• Selected contour(s): incremental offset from a Contour selected on the model.
• 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.
• Selected contour(s): incremental offset from a Contour selected on the model.
• 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.

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

• Clearance height: incremental offset from the Clearance Height.
• Retract height: incremental offset from the Retract Height.
• Disabled: disabling the Feed Height causes the tool to rapid down to the lead-in.
• 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.
• Selected contour(s): incremental offset from a Contour selected on the model.
• 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.

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

• 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.
• Selected contour(s): incremental offset from a Contour selected on the model.
• 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.
• Selected contour(s): incremental offset from a Contour selected on the model.
• 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.

Pass Direction

Specifies the cutting direction of the first passes.

Pass direction @ 0°

Pass direction @ 45°

Pass Extension

Distance to extend the passes beyond the machining boundary.

Pass extension

Stock Offset

Specifies the distance to offset the stock contour outwards.

Stock offset

Stepover

Specifies cutting stepover between passes. By default this value is 95% of the cutter diameter less the tool corner radius.

Stepover distance

Direction

The Direction option lets you control the cutting method. The default is to cut Both Ways, back and forth across the face. You may choose to cut in 1 direction by selecting either Climb or Conventional milling.

Both Ways - Cut in both directions (default) Climb - One direction Climb cut Conventional - One direction Conventional cut

From Other Side

Enable to start the toolpath on the other side of the part.

Unselected

Selected

Use Chip Thinning

Enable to use a roll-on cut to keep the chips thin.

Multiple Depths

Enable to create multiple depth cuts in the Z direction.

With Multiple Depth cuts

Without Multiple Depth cuts

Maximum Stepdown

Specifies the distance for the maximum stepdown between Z-levels. The maximum stepdown is applied to the full depth, less any remaining stock and finish pass amounts.

• The final pass may be less than the Max Stepdown.
• Shown without finishing stepdown.

Both Sides

Enable to machine from both side of the part when multiple depth cuts are taken. The starting stepover is applied from each side of the part for each stepdown pass.

Pass 1 starts on the right - Pass 2 starts on the left Pass 1 Stepover Distance measured from the right Pass 2 Stepover Distance measured from the left

Finishing Step

Enable to machine a finishing step in the Z axis.

Finishing step

Finish Feedrate

Feedrate used for the final finishing pass.

Finishing Stepdown

The amount for the Z finishing passes.

Finishing stepdown

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.

Axial (floor) Stock to Leave

The Axial Stock to Leave parameter controls the amount of material to leave in the axial (along the Z-axis) direction, i.e. at the end of the tool.

Radial stock to leave

Radial and axial stock to leave

Specifying a positive axial stock to leave results in material being left on the shallow areas of the part.

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

Allow Rapid Retract

When enabled, retracts are done as rapid movements (G0). Disable to force retracts at lead-out feedrate.

Keep Tool Down

When enabled, the strategy avoids retracting when the distance to the next area is below the specified stay-down distance.

Maximum Stay-Down Distance

Specifies the maximum distance allowed for stay-down moves.

Full Retract

Minimum Retract

Extend Before Retract

Enable to extend the cutting pass beyond the stock before retracting.

Lead-In (Entry)

Enable to generate a lead-in.

Lead-in

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

Lead-Out (Exit)

Enable to generate a lead-out.

Lead-out

Same as Lead-In

Specifies that the lead-out definition should be identical to the lead-in definition.

Vertical Lead-Out Radius

Specifies the radius of the vertical lead-out.

Vertical lead-out radius

Transition Type

Specifies the type of connection between passes.

Smooth Transition - between passes Straight Transition - between passes Short Transition - between passes No Contact (not shown) Passes are not connected on the same Z level. The tool retracts between each connecting pass.