About 2D Contour



Access:

Ribbon: CAM tab 2D Milling panel 2D Contour

The 2D Contour strategy lets you choose input geometry from 2D sketches, or by selecting faces from part geometry. The strategy then works on the edges of the selected faces by projecting the edges to the tool plane. Please note that this strategy, like all 2D operations, is not gouge-protected and the tool can gouge any surfaces or solids. It is your responsibility to ensure that the resulting toolpath produces the desired result.

Tool tab settings



Coolant:

The type of coolant used with the tool.

Spindle speed:

The rotational speed of the spindle.

Surface speed:

The spindle speed expressed as the speed of the tool on the surface.

Ramp spindle speed:

The rotational speed of the spindle when performing ramp movements.

Cutting feedrate:

Feed used in cutting moves.

Feed per tooth:

The cutting feedrate expressed as the feed per tooth.

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



Tangential extension distance:

Specifies the distance to extend the open contours tangentially.



No Tangential extension



10 mm Tangential extension

Separate tangential end extension

Enable to enter a tangential end extension distance value.

Tangential end extension distance:

Specifies the distance to extend the open contours tangentially at the end.

Stock Contours

Enable to specify the perimeter of the stock that needs to be faced.

Tabs

You can add tabs to the 2D Contour toolpath to hold the workpiece securely while all other material is machined away. Tabs are very useful when cutting thin plastic or wood materials using 2D routers.



Rectangular tabs



Triangular tabs

Rest Machining

Limits the operation to just remove material that a previous tool or operation could not remove.



Rest Machining ON



Rest Machining OFF

Tool diameter:

Specifies the diameter of the rest material tool.

Corner radius:

Specifies the corner radius of the rest material tool.

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:

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.

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

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

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 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 HSM 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.

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.

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.

Compensation type:

Specifies the compensation type.

Note: Control compensation (including Wear and Inverse wear) is only done on finishing passes.

Compensation radius allowance:

This parameter specifies a range of tool diameters that can be safely used, instead of only the tool selected for the operation.

The allowed range of tool radii start from the selected tool radius and goes up to the selected tool radius, plus the given allowance.

Make sharp corners

Specifies that sharp corners must be forced.

Caution: Using a smaller tool on the machine can cause a gouge when using this feature.

Finishing smoothing deviation:

The maximum amount of smoothing applied to the finishing passes. Use this parameter to avoid sharp corners in the toolpath. Setting this parameter leaves more stock than requested at the contour corners.



Multiple finishing passes

Enable to perform multiple finishing passes.

Number of finishing passes:

Specifies the number of finishing passes.



Shown with three finishing passes

Stepover:

The maximum distance between finishing passes.

Leads on all finishing passes

Forces a full lead in and out on every finishing pass.



Enabled



Disabled

Note: Lead parameters are set on the Linking tab.

Finish feedrate:

Feedrate used for the final finishing pass.

Repeat finishing pass

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

Finishing overlap:

The finishing overlap is the distance that the tool passes beyond the entry point before leading out. Specifying a finishing overlap ensures that the material at the entry point is properly cleared.



No finishing overlap



0.25" finishing overlap

Note: The finishing overlap follows the selected contour, so it is safe to specify a large overlap.

Lead end distance:

Specifies the distance the lead-out feed rate begins before the end of the selected geometry.



@ 0"



@ .5"

Note: This option is used when you desire to change the feedrate prior to breaking through at the end of the cut.

Outer corner mode

When machining outer corners, it may be necessary to avoid rolling around the corner in order to leave the corner perfectly sharp.

The Outer corner mode setting lets you machine outer corners in three different ways.

Tangential fragment extension distance:

Specifies the tangential extension of the passes.

Preserve order

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

Both ways

Specifies that the operation will use 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.

Roughing Passes

Enable to perform roughing passes.

Maximum stepover:

Specifies the maximum stepover.

Minimum cutting radius:



With Minimum cutting radius set

With Minimum cutting radius set - sharp corners in the toolpath are avoided minimizing chatter in finished parts.



Without Minimum cutting radius set

Without Minimum cutting radius set - the toolpath attempts to remove material anywhere the selected tool can reach. This produces sharp corners in the toolpath that often leads to chatter in the machined part.

Note: Setting this parameter leaves more material in internal corners requiring subsequent rest machining operations with a smaller tool.

Smoothing deviation:

The maximum amount of smoothing applied to the roughing passes. Use this parameter to avoid sharp corners in the toolpath.



Number of stepovers:

The number of roughing steps.

Multiple Depths

Specifies that multiple depths should be taken.



With Multiple Depth cuts



Without Multiple Depth cuts

Note: Adaptive clearing strategies allow from much more aggressive depth cuts than legacy 2D pockets.

Maximum roughing 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.

Finishing stepdowns:

The number of finishing passes using the bottom of the tool.



Shown with three finishing passes

Finishing stepdown:

The size of each stepdown in the finishing passes.



Finishing stepdown

Wall taper angle (deg):

Specifies the taper angle of the walls.

Defining a slope angle can be used to machine features with a 2D strategy that would have otherwise required a 3D strategy.

Note: The slope angle is NOT driven by model geometry so it is possible that an error entering the slope angle can affect the finish machined part.


Slope angle @ 0 degrees



Slope angle @ 45 degrees

Geometry Selection



Bottom Selection



Top Selection

Note: When using a slope angle with the Adaptive Clearing strategy, geometry must be selected at the top of the pocket.

Finish only at final depth

Perform finishing passes only at the final depth to avoid leaving marks on the walls.



Disabled



Enabled

Rough final

Enable to apply a finishing stepdown to every roughing pass/finishing pass when doing multiple depths with one or more finishing stepdowns.

Use even stepdowns

Enable to create equal distances between machining passes.

Example: Suppose you are machining a profile with a depth of 23 mm and a maximum stepdown = 10 mm.

Order by depth

Specifies that the passes should be ordered top down.



Disabled



Enabled

Order by islands

Specifies in which order the depth cuts are taken when there are multiple profiles.



Disabled

Disabled - Depth cuts are ordered by depth.



Enabled

Enabled - Depth cuts are ordered by profile.

Note: Ordering cuts by island minimizes the number of rapid moves.

Order by step

When enabled, each roughing and finishing step is machined to the full depth before moving to the next step.



Disabled



Enabled

Use thin wall

When milling part features with wall thicknesses comparable to sheet metal stock, or even thinner, the stock is subjected to the forces generated by metal removal. This can result in the delicate structure of thin walls moving relative to the tool, making it difficult to maintain dimensional accuracy and impart the specified surface finish.

This option can be used to reduce the vibration and chatter by ensuring that both sides of a thin wall are machined at the same time.

Thin wall width:

The width of walls that should be considered thin walls.

Any wall with this width (or thinner) is machined on both sides at the same time to reduce vibration and chatter.

Chamfer

Specifies that the contouring operation is to be used to create a chamfer.

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 edges selected must be either at the bottom edge of a chamfered face or unchamfered edges. If both edge types are selected, then the edges that already have the chamfers modeled will end up with chamfers that are twice the size they should be.

Chamfer width:

The (additional) width of the chamfer.

For edges that are not already chamfered, this is the final width of the chamfer.

For chamfered edges, this is an additional offset; similar to using negative radial stock to leave.

Chamfer tip offset:

This is added to the toolpath depth, while keeping the tool in contact with the selected edge by adjusting the toolpath radial offset.

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, Inventor HSM 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 HSM 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



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 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.

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

Lift height:

Specifies the lift distance during repositioning moves.



Lift height 0



Lift height .1 in

Lead-in (entry)

Enable to generate a lead-in.



Lead-in

Horizontal lead-in radius:

Specifies the radius for horizontal lead-in moves.



Horizontal lead-in radius

Lead-in sweep angle:

Specifies the sweep of the lead-in arc.



Sweep angle @ 90 degrees



Sweep angle @ 45 degrees

Linear lead-in distance:

Specifies the length of the linear lead-in move for which to activate radius compensation in the controller.



Linear lead-in distance

Perpendicular

Replaces tangential extensions of lead-in/lead-out arcs with a move perpendicular to the arc.



Shown with Perpendicular entry/exit

Example: A bore with lead arcs that are as large as possible (the larger the arc the less chance of dwell mark), and where a tangent linear lead is not possible because it would extend into the side of the bore.

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.

Linear lead-out distance:

Specifies the length of the linear lead-out move for which to deactivate radius compensation in the controller.



Linear lead-out distance

Horizontal lead-out radius:

Specifies the radius for horizontal lead-out moves.



Horizontal lead-out radius

Vertical lead-out radius:

Specifies the radius of the vertical lead-out.



Vertical lead-out radius

Lead-out sweep angle:

Specifies the sweep of the lead-out arc.

Perpendicular

Replaces tangential extensions of lead-in/lead-out arcs with a move perpendicular to the arc.



Shown with Perpendicular entry/exit

Example: A bore with lead arcs that are as large as possible (the larger the arc the less chance of dwell mark),and where a tangent linear lead is not possible because it would extend into the side of the bore.

Ramp

Enable ramps.



Shown with a 15 degree Ramping angle

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.

Helical ramp diameter:

Specifies the helical ramp diameter.

Minimum ramp diameter:

Specifies the minimum ramp diameter.

Predrill positions

Select points where holes have been drilled to provide clearance for the cutter to enter the material.

Entry positions

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

Predrill positions

Select points where holes have been drilled to provide clearance for the cutter to enter the material.

Entry positions

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

Topics in this section
Parent topic: About 2D Milling