Trace

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.

Access:

Ribbon: CAM tab 2D Milling panel Trace

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.

Geometry tab settings

Geometry

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

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.

Axial Offset Passes shown.

Tool Orientation

Not available in Inventor CAM Express

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:

The Origin drop-down menu offers the following options for locating 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

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

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

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

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, CAM 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 Inventor CAM 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

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, Inventor CAM 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.

Axial Offset Passes

Enable to do multiple depth cuts.

Axial offset passes are used to create multiple incremental Z passes in many of the 3D finishing strategies. They work much like multiple finishing stepdowns in the 2D operations and are useful for removing a fixed amount of stock using several passes.

Shown with 4 cuts of .010 in



Three axial offset passes

Maximum stepdown:

Specifies the maximum stepdown between Z-levels for roughing.



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.

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.



Don't Care



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.

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.

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, Inventor CAM 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, Inventor CAM 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

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.
Caution: 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).

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.

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.



1" Maximum stay-down



2" Maximum stay-down distance

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