Flat Finishing reference

Automatically detects the flat areas of the part for machining.

Manufacture > Milling > 3D > Flat

This strategy detects all the flat areas of the part and clears them with an offsetting path similar to the Pocket Clearing or a 2D Face strategy. There is an option to cut down to the horizontal face in stages, which means this strategy can be used as a semi-roughing and finishing toolpath.

When the flat area is shelved above the surrounding areas, the cutter moves beyond the flat areas to clean the edges.

Tool tab settings

Tool

Press Select to access the tool library. See the reference documentation on Tool Library for more information on selecting tools.

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.

• Preset - Select the predefined Cutting Date for the selected tool, to set the speeds and feeds
• 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

Shaft & Holder

When enabled, this provides additional controls for collision handling. Collision detection can be done for both the tool shaft and holder, and they can be given separate clearances. Choose between several modes, depending on the machining strategy.

This function increases the number of calculations that need to be performed. This may effect the performance of your system on very large projects.

Shaft and Holder Modes

Disabled		Pull away
Does not calculate for any shaft/holder collisions.		Pulls the toolpath away from the workpiece to maintain a safe distance between the shaft and/or holder.
Trimmed		Detect tool length
Reduces the travel of the cut to avoid a collision with the holder.		Automatically extended the tool further out of the holder to maintain the specified safe distance between the shaft and/or holder and the workpiece. A message indicating how the far the tool is extended out of the holder is logged.

Fail on collision - The toolpath calculation is aborted and an error message logged when the safe distance is violated.

Settings

• Use Shaft - Enable to include the shaft of the selected tool, in the toolpath calculation, to avoid collisions.
• Shaft Clearance - The tool shaft always stays this distance from the part.
• Use Holder - Enable to include the holder of the selected tool, in the toolpath calculation, to avoid collisions.
• Holder Clearance - The tool holder always stays this distance from the part.

Geometry tab settings

Machining Boundary

Machining Boundary specifies how the toolpath boundary is defined. The following images are shown using a 3D Radial toolpath.

Silhouette		Selection

Boundary modes:

Bounding box	Silhouette	Selection
Defined by the rectangular extents of the part as viewed from the WCS tool plane view (Top)	Defined by the shadow edge of the part profile as viewed from the WCS tool plane view (Top)	Defined by a selection that can be edges of the model or a sketch boundary.

None - Defined by the stock size specified in the Setup. Not available for all machining strategies.

Tool Containment

Use tool containment to control the tools position in relation to the selected boundary or boundaries.

Tool inside boundary	Tool center on boundary	Tool outside boundary
The entire tool stays inside the boundary. As a result, the entire surface contained by the boundary might not be machined.	The boundary limits the center of the tool. This setting ensures that the entire surface inside the boundary is machined. However, areas outside the boundary or boundaries might also be machined.	The toolpath is created inside the boundary, but the tool edge can move on the outside edge of the boundary.

Additional Offset

An additional offset can be applied to the selected boundary/boundaries and tool containment. A positive value offsets the boundary outwards unless the tool containment is Inside, in which case a positive value offsets inwards.

Examples shown with Tool Containment set to Tool center on boundary.

Negative offset	No offset	Positive offset
Tool is offset inside	Tool stays on the boundary	Tool is offset outside

To ensure that the edge of the tool overlaps the boundary, select the Outside tool containment method and specify a small positive value.

To ensure that the edge of the tool is completely clear of the boundary, select the Inside tool containment method and specify a small positive value.

Contact Point Boundary

When enabled, extends the Machining boundary limits of the cut position to where the tool touches the part, rather than the tools center position. In the illustration below the red line indicates the machining boundary edge selection, as viewed through the tool plane. The blue line indicates the tool contact point.

The difference is illustrated below on a Parallel toolpath using a ball end mill.

Disabled		Enabled

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.

Model

Enable to override the model geometry (surfaces/bodies) defined in the setup.

Include Setup Model

Enabled by default, the model selected in the setup is included in addition to the model surfaces selected in the operation. If you disable this checkbox, then the toolpath is generated only on the surfaces selected in the operation.

Avoid/Touch Surfaces

When enabled, select the surfaces to avoid. The tool must avoid the selected surfaces by the specified amount.

Disabled		Enabled

Avoid/Touch Surface Clearance

Set the distance for the tool to avoid the selected surfaces.

Touch Surfaces

Inverts the meaning of the Avoid surfaces setting. When enabled, the avoid surfaces are the ones that must be touched within the given clearance while the remaining surfaces are avoided.

Touch surfaces enabled

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.
• 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.
• 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.
• 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.
• 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.
• 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.
• 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.
• 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.
• 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 machining tolerance is the sum of the tolerances used for toolpath generation and geometry triangulation. Any additional filtering tolerances must be added to this tolerance to get the total tolerance.

Loose Tolerance .100	Tight Tolerance .001

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.

Type

Generates a style of toolpath that resembles either the Pocket or Parallel strategy.

Pocket		Parallel
Useful for machining complex geometry, such as multiple circular regions. Passes are offset from one another. Options are available to optimize the toolpath over open pockets and generate a spiral-style toolpath for continuous machining.		Useful for machining simpler geometry, such as long rectangular regions. Passes are arranged in straight lines and do not have corners. Corners in the toolpath often slow down the machine and may cause marks on the surface.

Optimize Open Pockets

When enabled the tool will approach from the open sides of a pocket. This results in more efficient entry moves such as a short tangential extension instead of a ramp move, and better cutting conditions.

• Reduces full-width tool cuts.
• Reduces sharp corners in the toolpath.

When disabled, the tool is restricted from entering the cut area from outside of the part. This can be useful to avoid clamps or fixtures that may be in the way. There are also less tool-lifts, which makes it faster for machining softer materials like foam, where the cutting conditions are not as critical.

Enabled		Disabled
Cuts moves can overlap the edge of the cut area.		Cut moves are contained within the cut area.

Continuous

Generates a spiral-style toolpath that has minimal link moves between passes, resulting in a better surface finish.

Enabled		Disabled

Stepover

The stepover distance between cuts.

Smoothing Deviation (%)

A sliding scale adjustment between 0% and 25% percent, that represents a deviation of the actual stepover path. This creates a fluid motion for the machining path, to reduce sharp corners.

The smoothing deviation applies to inner cuts and does not affect the accuracy of the final profile cut.

0% Deviation		25% Deviation

Profile Cut Direction

The Profile Cut Direction lets you control if Fusion should create a Climb cut Conventional cut or cut Both Ways across the surface.

		1 - Climb cut 2 - Conventional Cut 3 - Both Ways

Cut Interior Both Ways

When enabled this alternates between climb and conventional cuts for all interior passes. The final cut is controlled by the Profile Cut Direction setting (illustrated by the orange arrow).

When disabled, the Profile Cut Direction determines the direction of all cuts.

Enabled		Disabled

Finishing Pass

When enabled this allows you to add a finish pass for the final stepover.

The final stepover is where the tool engages the floor but also nearby side walls. Having an additional pass helps give a finer cut and a better surface finish.

Enabled		Disabled

Finishing Stepover

The distance for the final passes, which is typically smaller than the stepover value.

Machine Over Holes

When enabled the toolpath continues across holes rather than going around the opening. The continuous motion creates a more uniform toolpath across the flat area and eleminates the need to patch the open hole areas.

This results in fewer changes in direction, resulting in a better surface finish and possibly a reduced cycle time.

Enabled		Disabled

Max Hole Size

Machines over holes that are smaller than the specified hole diameter.

In the example below, the hole on the top has a 30 mm diameter and the hole on the bottom has a 50 mm diameter.

Entering a Max Hole Size value of 40 mm means a toolpath is generated over the top hole and nothing is generated over the bottom hole.

Multiple Depths

Enable to do multiple depth cuts. Multiple Depths is useful for removing a fixed amount of stock by creating multiple incremental Z offset passes. This is available in many of the 3D finishing strategies.The following images are shown with 3D Parallel.

Disabled		Enabled
Single Z depth pass		Shown with three Z passes

Total Depth

The total amount of stock to remove from the surface.

Maximum Stepdown

The amount to stepdown between Z-levels cuts.

Finishing Stepdown

The amount to stepdown for the final Z-level cut.

Stock to Leave

A positive stock value leaves material for subsequent roughing or finishing operations. Roughing operations generally leave a small amount of material for a precision finish cut.

A negative stock value 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.

A zero stock amount (0.0) value remove all excess material up to the selected geometry.

Positive	No Stock	Negative

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.

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 bottom of the tool.

Radial - Wall stock	Radial and Axial	Axial - Floor stock

For surfaces that are not exactly vertical, Fusion interpolates between the axial (floor) and radial (wall) 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.

When using a ball or radius cutter, the negative axial stock must be less than or equal to the corner radius of the selected tool.

Fillets

Enable to enter a fillet radius.

Fillet Radius

Specify a fillet radius.

Smoothing

Smooths the toolpath by removing excessive points and fitting arcs where possible within the given filtering tolerance.

Smoothing Off	Smoothing On

Smoothing is used to reduce code size without sacrificing accuracy. Smoothing works by replacing collinear lines with one line and tangent arcs to replace multiple lines in curved areas.

The effects of smoothing can be dramatic. G-code file size may be reduced by as much as 50% or more. The machine will run faster and more smoothly and surface finish improves. The amount of code reduction depends on how well the toolpath lends itself to smoothing. Toolpaths that lay primarily in a major plane (XY, XZ, YZ), like parallel paths, filter well. Those that do not, such as 3D Scallop, are reduced less.

Smoothing Tolerance

Specifies the smoothing filter tolerance.

Smoothing works best when the Tolerance (the accuracy with which the original linearized path is generated) is equal to or greater than the Smoothing (line arc fitting) tolerance.

Feed Optimization

Specifies that the feed should be reduced at corners.

Maximum Directional Change - Specifies the maximum angular change allowed before the feedrate is reduced.

Reduced Feed Radius - Specifies the minimum radius allowed before the feed is reduced.

Reduced Feed Distance - Specifies the distance to reduce the feed before a corner.

Reduced Feedrate - Specifies the reduced feedrate to be used at corners.

Only Inner Corners - Enable to only reduce the feedrate on inner corners. Enable to only reduce the feedrate on inner corners.

Linking tab settings

Retraction Policy

Controls how the tool moves between cutting passes. The following images are shown using the Flow strategy.

• Full retraction - completely retracts the tool to the Retract Height at the end of the pass before moving above the start of the next pass.

• Minimum retraction - moves straight up to the lowest height where the tool clears the workpiece, plus any specified safe distance.

• Shortest path - moves the tool the shortest possible distance in a straight line between paths.

Full Retract	Minimum Retraction	Shortest Path

For CNC machines that do not support linearized rapid moves, the post processor can be modified to convert all G0 moves to high-feed G1 moves. Contact technical support for more information or instructions how to modify post processors as described.

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.

Leads and Transitions

These parameters control how the toolpath should lead into and lead off-of the toolpath cuts. This consist of a combination of linear and circular motion.

Lead In Moves

Vertical Lead-In Radius		Lead-In Linear Move
The radius of the vertical arc for smoothing the entry into the toolpath.		The linear distance for smoothing the entry into the toolpath.

Lead Out Moves

Vertical Lead-Out Radius		Lead-Out Linear Move
The radius of the vertical arc for smoothing the exit off of the toolpath.		The linear distance for smoothing the exit off of the toolpath.

Ramp Type

Specifies how the cutter enters the part for each depth cut.

Plunge Outside Stock		Predrill
Plunge		Zigzag
Profile		Smooth Profile
Helix

Ramping Angle (deg)

Specifies the maximum ramping angle.

Maximum Ramp Stepdown

Specifies the maximum stepdown per revolution on the ramping profile. This parameter allows the tool load to be constrained when doing full-width cuts during ramping.

Ramp Clearance Height

Height of ramp over the current stock level.

Ramp Radial Clearance

Specifies the minimum distance to the contour for the lead-in helix.

Helical Ramp Diameter

Specifies the helical ramp diameter.

Minimum Ramp Diameter

Specifies the minimum ramp diameter.

Predrill positions

If Predrill is selected use this to specify the location of the hole. Fusion assumes you drilled a hole at this location.

Entry positions

Selection an entry positions for the start of the ramp.