Slot reference

Slot mills a centerline path by selecting Edges or Sketches. It does not contour the perimeter of the selected slot. The tool should be the width of the actual slot or smaller. The Slot shape can be open or closed, straight, circular or contain multiple curves. But it must be a continuous width slot shape. Useful for clearing a channel before machining a boundary.

Manufacture > Milling > 2D > Slot

The animation below shows a slot that has a width of 10 mm. The slot is machined by a 10 mm diameter tool.

slot animation

The default settings for Slot allow it to ramp to the final depth. Select the lower edge or sketch that represents the slot.

Geometry selection for a Slot operation

Toolpath generated for the selected geometry

Tool tab settings

2d slot 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 slot dialog geometry tab

Geometry

Slot can be used on any Edge or Sketch that represents a slot shape.

2d slot many chains example

Note: The Slot toolpath will only cut a clearance channel thru the center. It is not an area clearance toolpath like 2D Offset Roughing or 2D Adaptive Roughing.

Pocket Selection

Closed or open boundaries can be machined by selecting Edges or Sketches. The Slot shape can be straight, circular or contain multiple curves. But it must be a continuous width slot shape.

Geometry selection for a Slot operation

Toolpath generated for the selected geometry

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 slot dialog heights tab

For machining heights, see Setting machining heights and:

Passes tab settings

2d slot 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.

Backoff Distance

After reaching the end of the cut, the tool will back off from the wall before retracting.

Backoff set to 0.0

Backoff set to .25

Repeat Finishing Pass

When checked the tool makes an additional cut to remove any stock left from tool deflection.

Finish Pass Disabled

Finish Pass Enabled

Tangential Fragment Extension Distance

Specifies the tangential extension of the passes on open slots

Preserve Order

When checked the features are machined in the order they were selected. When unchecked the toolpath order is optimized for the most efficient path.

Multiple Depths

The default for Slot is to ramp to the depth. This will zig-zag to the full depth. One way to reduce the tool load is to take multiple depth cuts.

No Multiple Depth cuts.

Multiple Depths (blue line)

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.

Axial (floor) Stock to Leave

Controls the amount of material to leave in the axial direction (along the Z-axis), i.e. at the end of the tool. Using a negative stock value removes more material from the floor of the slot.

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 slot dialog linking tab

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 only (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 rapid 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.

Maximum Stay-Down Distance

Specifies the maximum distance allowed for stay-down moves.

1" Maximum stay-down

2" Maximum stay-down distance

Ramp Type

Specifies how the cutter moves down for each depth cut.

Predrill.	Predrill Point Location.
Plunge at start of cut.
Profile.	Profile follows the slot shape. This is the default Ramp Type. The tool will ramp at the specified angle for the length of the slot. Reaching the full depth may require multiple zip-zag ramp moves. You can limit the depth of the ramp using the Maximum Ramp Stepdown

Ramping Angle (deg)

Specifies the maximum ramping angle. If Ramp Type is set to Profile, the tool will ramp at the specified angle for the length of the slot.

Maximum Ramp Stepdown

Specifies the maximum ramping depth when using the Profile - Ramp Type on long slots. This will limit the tool load for very deep or very short slots.

.750" Maximum Ramp Stepdown

.300" Maximum Ramp Stepdown

Ramp Clearance Height

The height over the stock where the ramp toolpath start.

Predrill Positions

Select the points where holes have been drilled to provide clearance for the cutter to enter the material. Used with Predrill - Ramp Type.

Predrill Point Location.

Plunge starts at Predrill point.

Entry Positions

Select geometry near the location where you want the tool to enter.