Morphed Spiral reference

Morphed Spiral can be very useful when machining free-form/organic surfaces.

morphed spiral strategy

Manufacture > Milling > 3D > Morphed Spiral

The Morphed Spiral strategy is very similar to the Spiral strategy. However, a Morphed Spiral operation generates the spiral from the selected boundary as opposed to a Spiral operation which trims the generated passes to the machining boundary. This means that Morphed Spiral can be used for additional surfaces for which Spiral is not appropriate.

Morphed Spiral can be very useful when machining free-form/organic surfaces. Although the Scallop strategy is often used for these types of surfaces, both the sharp corners and the linking transitions between the generated passes can result in visible marks. The Morphed Spiral strategy generally provides a much smoother toolpath by avoiding these issues.

morphed spiral strategy Although a Scallop strategy is often used to machine free-form/organic surfaces...

morphed spiral strategy ...a Morphed Spiral strategy provides a much smoother toolpath avoiding visible marks.

Important: Since Morphed Spiral is not appropriate for steep areas, it is recommended that you use Scallop or one of the other strategies for steep area machining.

Tool tab settings

3d morph spiral 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.

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 - When Shaft and Holder is disabled Fusion does not calculate for any shaft/holder collisions.

shaft and holder mode diagram - disabled

Pull away - The toolpath pulls away from the workpiece to maintain a safe distance between the shaft and/or holder.

shaft and holder mode diagram - pull away

Detect tool length - The tool is automatically extended 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.

shaft and holder mode diagram - detect length

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

3d morph spiral dialog geometry tab

Machining Boundary

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

radial boundary mode diagram Example 1

radial boundary mode diagram Example 2

Boundary modes:

None - The toolpaths machine all stock without limitation.
Bounding box - Contains toolpaths within a box defined by the maximum extents of the part as viewed from the WCS.

Bounding box

Silhouette - Contains toolpaths within a boundary defined by the part shadow as viewed from the WCS.

Silhouette

Selection - Contains toolpaths within a region specified by a selected boundary.

Selection

Tool Containment

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

Inside

The entire tool stays inside the boundary. As a result, the entire surface contained by the boundary might not be machined.

tool containment diagram - inside Inside

Center

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.

tool containment diagram - center Center

Outside

The toolpath is created inside the boundary, but the tool edge can move on the outside edge of the boundary.

tool containment diagram - outside Outside

To offset the boundary containment, use the Additional Offset parameter.

Additional Offset

The additional offset is 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.

boundary offset diagram - inward Negative offset with tool center on boundary

boundary offset diagram - none No offset with tool center on boundary

boundary offset diagram - outward Positive offset with tool center on boundary

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, specifies that the boundary limits where the tool touches the part rather than the tool center location.

contact point boundary diagram - disabled Disabled

contact point boundary diagram - enabled Enabled

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

contact point boundary parallel diagram - enabled Disabled

contact point boundary parallel diagram - disabled Enabled

Contact Only

Controls whether or not toolpaths are generated where the tool is not in contact with the machining surface. When disabled, toolpaths are extended to the limits of the containment boundary and across openings in the workpiece.

contact only diagram Enabled

contact only diagram Disabled

Slope

Contains toolpaths based on a range of specified angles.

slope containment diagram - 0-90 degrees 0° - 90°

slope containment diagram - 0-45 degrees 0° - 45°

slope containment diagram - 45-90 degrees 45° - 90°

Slope angle confinement is specified by the From Slope Angle and To Slope Angle angle parameters on the Geometry tab. Angles are defined from 0° (horizontal) to 90° (vertical).

Only areas equal to or greater than the values in the From Slope Angle and To Slope Angle parameters are machined.

Most 3D finishing strategies support slope angle confinement. One use of slope confinement is to confine a selected toolpath strategy to angles where it works best. For example, Parallel Finish is better suited to shallow areas while Contour Finish is better suited to steep areas.

From Slope Angle

From Slope Angle is defined from the 0° (horizontal) plane. Only areas equal to or greater than this value are machined.

from slope angle diagram Slope angle from 0°

To Slope Angle

To Slope Angle is defined from the 0° (horizontal) plane. Only areas equal to or less than this value are machined.

to slope angle diagram Slope angle to 90°

Rest Machining

When checked this limits the operation to only remove material that a previous tool or operation could not remove.

Rest stands for REmaining STock.

Area to Machine - Pocket shown in green.
Previous Operation - Not all stock is removed.
Rest Machining Off - All areas are machined.
Rest Machining On - Previously un-cut areas are machined.

Source

Specifies the source from which the rest machining is to be calculated.

From previous operation(s)
From tool
From solid(s)
From setup stock

From Setup Stock

Uses the stock body as defined in the Setup

Tool Diameter

Specifies the diameter of the rest material tool.

Corner Radius

Specifies the corner radius of the rest material tool.

Taper Angle

Specifies the rest material tool taper angle.

Shoulder Length

Specifies the rest material tool shoulder length.

Ignore Stock Less Than

Specifies the amount of stock from previous operations to ignore. Expressed in distance units. The parameter helps you avoid machining of minor rest material.

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

Specifies surfaces to avoid. When enabled, toolpaths stay away from the selected surfaces by a specified amount.

avoid surfaces diagram - disabled Disabled

avoid surfaces diagram - enabled Enabled

Avoid/Touch Surface Clearance

The tool always stays this distance from 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 diagram Touch surfaces

Heights tab settings

3d morph spiral 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

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.
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 diagram 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.
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 diagram 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.
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 diagram 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.
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

3d morph spiral dialog passes tab

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.

Inside/Outside Direction

Specifies if the toolpath moves inside-out or outside-in. Selecting the Shortest machining distance option uses a mixture of the ordering to achieve the shortest machining distance.

Inside > out

Outside > in

Clockwise

Specifies that the spiral is clockwise.

Stepover

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

horizontal stepover diagram Horizontal stepover

Direction

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

direction diagram - one way Climb

direction diagram - both ways Both Ways

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.

Conventional

This reverses the direction of the toolpath compared to the Climb setting to generate a conventional milling toolpath.

Both Ways

When Both ways is selected, Fusion disregards the machining direction and links passes with the directions that result in the shortest toolpath.

Multiple Depths

Enable to do multiple depth cuts.

Multiple Depths are used to create multiple incremental Z offset passes in many of the 3D finishing strategies and are useful for removing a fixed amount of stock using several passes. The following images are shown with 3D Parallel.

axial offset pass diagram - single pass Disabled

axial offset pass diagram - 3 passes three stepdowns

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.

stepdown max

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

Number of Stepdowns

Specifies the desired number of stepdowns.

Order by Depth

When enabled, this orders the cuts of multiple contours or cavities by Z level.



Model with multiple cavity selections	All cavities cut by Z level

Up/Down Milling

Use this option to break each pass into segments so that each piece is machined using either downward or upward moves only. This is useful when using insert cutters that are restricted to a specific cutting direction.

up down milling diagram Both

down milling diagram Down Milling

Stock to Leave

stock to leave diagram - positive 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.

stock to leave diagram - none None

No Stock to Leave - Remove all excess material up to the selected geometry.

stock to leave diagram - negative 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.

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.

stock to leave diagram - radial Radial stock to leave

stock to leave diagram - both 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.

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.

stock to leave diagram - axial Axial stock to leave

stock to leave diagram - both Both 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.

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.

Note: Total tolerance, or the distance the toolpath can stray from the ideal spline or surface shape, is the sum of the cut Tolerance and Smoothing Tolerance. For example, setting a cut Tolerance of .0004 in and Smoothing Tolerance of .0004 in means the toolpath can vary from the original spline or surface by as much as .0008 in from the ideal path.

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.

Linking tab settings

3d morph spiral dialog linking tab

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.

Important: The Shortest path option should not be used on machines that do not support linearized rapid movements where G0 moves are straight-line (versus G0 moves that drive all axes at maximum speed, sometimes referred to as "dogleg" moves). Failure to obey this rule will result in machine motion that cannot be properly simulated by the software and may result in tool crashes.

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.

Allow Rapid Retract

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

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.