Trace reference

Trace allows you to machine 3D Edge contours. You can select Edges from the model or Sketch geometry. This single line engraving can be used for scroll work or text. You can machine on center or use left and right compensation. Using left and right compensation might create disconnected passes at the corners due to sudden changes in the Z position.

2d trace oil groove toolpath example

Manufacture > Milling > 2D > Trace

Tool tab settings

2d trace 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

Geometry tab settings

2d trace dialog geometry tab

Geometry

Select any 3D Edge or Sketch to define the machining curve.

2d trace oil groove toolpath example

Curve Selection

Select any 3D Edge or Sketch to define the machining curve. This edge can be used for single line engraving, text or edge cleanup by using the Chamfer options.

Cutting serrations on the face.

Multiple Depths shown.

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

2d trace 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.
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 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.
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.

Passes tab settings

2d trace dialog passes tab

Tolerance

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



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.

Pass Extension

Distance to extend the passes beyond the machining boundary.

pass extension diagram

Pass extension

Sideways Compensation

This setting determines the side of the toolpath from which the tool center is offset. Choose between Left (climb milling) sideways compensation or Right (conventional milling) sideways compensation.

Left (climb milling)

Climb Milling

Right (conventional milling)

Conventional Milling

Climb milling can be thought of as the cutter ''rolling along'' the surface that it is cutting. This generally gives a better finish in most metals, but requires good machine rigidity. Using this method, chips start at maximum thickness and get thinner towards the end of the cut, meaning more heat in the chip and less in the part.

With conventional milling, the cutter is ''rotating away'' from the surface it is cutting. This method is more commonly used with manual or less rigid machines. It does have some advantages, and can even give a better finish when machining certain materials including some woods.

Repeat Passes

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

Preserve Order

Specifies that features are machined in the order in which they were selected. When unselected, Fusion optimizes the cut order.

Both Ways

Specifies that the operation uses both Climb and Conventional milling to machine open profiles.

Unselected

Selected

Note: This option only controls how multiple depth cuts are taken on a single open contour. It does not optimize the cut direction for multiple open contours.

Maximum Angle (deg)

Limits the toolpath if the point of contact point slopes less than the angle specified.

Axial Offset

Can be used to shift the selected curve up or down in the spindle axis.

Multiple Depths

Enable to do multiple depth cuts.

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

Shown with 4 cuts of .010 in

three stepdowns

Maximum Stepdown

Specifies the maximum stepdown between Z-levels for roughing.

maximum stepdown diagram

Maximum stepdown - shown without finishing stepdowns

Note: Sequential Z-level stepdowns are taken at the Maximum stepdown value. The Final Roughing stepdown takes the remaining stock, once the remaining stock is less than the Maximum stepdown Value.

Number of Stepdowns

Specifies the desired number of stepdowns.

Order by Depth

This alters the order of the cuts when multiple curves are selected. When enabled, Order By Depth cuts all of a single curve before cutting the next curve.

order by depth with 2 edge curves example

Shown with 2 Edge Curves selected.

Enabled

Curve 1 is cut complete before curve 2.

Disabled

Toolpath is generated by level cutting both curves.

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.

Both

Down Milling

Chamfer

Only available if a Tapered or Chamfer tool is selected. Allows additional parameters to Chamfer a sharp edge, or a modeled Chamfer on the part.

Geometry Selection Tips:

Sharp Corners

Sharp Corners - Select the sharp corner and define the size of the chamfer using the Chamfer Width setting.

Chamfered Edges

Chamfered Edges - Select the bottom edge of the chamfer. The chamfer width is calculated automatically.

Note: All selected edges must be the same type. Select either a sharp unchamfered edge, or the bottom edge of a chamfered face. If both edge types are selected, the edges that already have chamfers modeled, will end up with chamfers that are twice the size they should be.

Chamfer width

The amount to adjust the chamfer size.

Chamfer width added to sharp edge

For sharp edge selections this is the final width of the chamfer
For chamfered edges selections this can add additional offset width to a modeled chamfer. Similar to using stock to leave

Chamfer tip offset

The amount to extend the tool tip past the edge of the chamfer.

chamfer tip offset diagram

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.

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.

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.

Axial stock to leave

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.

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

2d trace 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.

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.