2D Chamfer

The 2D Chamfer is used to create a beveled edge on the part. Select from Edges or Sketches. A tapered tool is required.

Access:

Ribbon: CAM tab 2D Milling panel 2D Chamfer

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

You can select Edges or Sketches. Contiguous geometry is automatically chained.

Contour Selections

Select the sharp edge on a part without modeled chamfers. If the Chamfer is modeled, select the lower edge of the chamfer.

Sharp Edge Selection.

Modeled Edge Selection.

Tangential Extension Distance

Used on open contours to extend the beginning and end of the selected chain or multiple chains. This creates a tangent linear extension based on the angle of the start and endpoints. This is an extension of the selected geometry.

  1. No Extension
  2. 12mm Extension
  3. Single pass - Long extension
  4. Multiple Finish Passes set to 2

If the extension distance causes an overlap of a single chain, the intersection will be trimmed into a closed boundary.

Note: You can use the Stock Contours option to force the toolpath past the defined Stock or a selected boundary. Great for irregular shapes. For an additional extension to the toolpath, go to the '''Passes Tab''' and use the '''Tangential Fragment Extension Distance

Separate Tangential End Extension

Enable this option to enter a different end extension length value.

Tangential End Extension Distance

Specifies the distance to extend the end position.

16mm Start Extension & 5mm End Extension

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:

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 check box, then the toolpath is generated only on the surfaces selected in the operation.

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 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.

Compensation type:

Specifies the compensation type.

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

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.

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 Clearance

This value specifies how far the tool needs to stay away from model geometry that is not being chamfered.

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.

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.

Horizontal lead-out radius:

Specifies the radius for horizontal lead-out moves.



Horizontal lead-out radius

Lead-out sweep angle:

Specifies the sweep of the lead-out arc.

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

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-out radius:

Specifies the radius of the vertical lead-out.



Vertical lead-out radius

Entry Positions

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

Parent topic: 2D Milling Functionality