Overview#
Face and 2D Contour are the two most common first operations on a plate or bar part.
- Face removes a thin layer from the top of the stock to create a flat, clean reference surface. It is usually the first operation in a Setup.
- 2D Contour moves a tool along a chain of edges or a sketch profile, cutting on the inside, outside, or on the line. It cuts outside profiles, internal profiles, steps and walls, and it can be used for both roughing (with multiple depths and stock to leave) and finishing.
Both belong to the 2.5D family: the tool moves in X and Y at a series of fixed Z levels. They are fast to program, predictable, and efficient.
This page covers the shared dialog structure of 2D operations (tabs Tool, Geometry, Heights, Passes, Linking) using Face and 2D Contour as examples. The next page extends this to offset and adaptive roughing.
Where to find it#
- Milling > 2D > Face
- Milling > 2D > 2D Contour
- Toolbar search (S), then type "Face" or "2D Contour"
The common dialog structure#
Most 2D operations present the same five tabs (some add a Rest/Chamfer or other group within them):
| Tab | What it holds |
|---|---|
| Tool | Tool selection, preset, spindle speed, feeds, coolant |
| Geometry | Which faces, edges or sketch curves define the toolpath; stock contours; tabs and rest machining where offered; tool orientation |
| Heights | The five heights (clearance, retract, feed, top, bottom) that define vertical movement |
| Passes | Tolerance, compensation, stepdowns, stepovers, finishing passes, stock to leave and strategy-specific choices |
| Linking | High feedrate mode, retracts and stay-down, lead-in/lead-out, ramps and transitions |
Understanding the Heights tab is critical for every operation.
The five heights#
| Height | Meaning |
|---|---|
| Clearance Height | The first height the tool rapids to on its way to the start of the toolpath |
| Retract Height | The height the tool moves up to before the next cutting pass; set above Feed height and Top |
| Feed Height | The height the tool rapids to before changing to the feed/plunge rate to enter the part; set above Top (can be Disabled, so the tool rapids down to the lead-in) |
| Top Height | The top of the cut; set above Bottom |
| Bottom Height | The final machining depth, the lowest point the tool descends to; set below Top |
Each height has a From reference and an Offset (positive or negative). Autodesk's lists of references include Stock top, Stock bottom, Model top, Model bottom, the other heights, and, for Retract, Feed, Top and Bottom, a Selection (point, edge or face on the model). A sensible arrangement is Top = Stock top, Bottom = Selection or Model bottom, with Feed, Retract and Clearance stepped up from Top by offsets you choose. Defaults vary by operation, so check the preview.
Heights are measured along the WCS Z, so a wrong WCS shows up here too.
Face#
Step by step#
- Create the Setup with a stock Top Offset of at least 1 mm (or the amount you plan to remove).
- Milling > 2D > Face.
- Tool: select a face mill (best) or a large end mill.
- Geometry: with no selection Fusion faces the stock defined in the Setup (the Face toolpath assumes you want to machine the top of the stock to Z0). To limit the area, select an edge or sketch boundary.
- Heights: Top is the stock top; Bottom is the finished face.
- Passes: choose Direction, Stepover, Pass Extension, Stock Offset, Multiple Depths and Stock to Leave.
- Linking: use the defaults, then adjust lead-in/out if needed.
- Click OK, then Generate and Simulate.
Face options of note#
| Option | What it does | Notes/default |
|---|---|---|
| Pass Direction | Angle of the first passes | e.g. 0 or 45 degrees |
| Pass Extension | Distance to extend passes beyond the machining boundary | Ensures complete coverage |
| Stock Offset | Offsets the stock contour outwards | |
| Stepover | Distance between passes | Default is 95% of the cutter diameter less the tool corner radius |
| Direction | Both Ways, Climb or Conventional | Default Both Ways |
| From Other Side | Starts on the other side of the part | |
| Use Chip Thinning | Roll-on cut to keep chips thin | |
| Multiple Depths / Maximum Stepdown | Z levels for heavy facing | The last pass may be smaller |
| Both Sides | With multiple depths, alternates the starting side | |
| Finishing Step / Finishing Stepdown / Finish Feedrate | A finishing pass in Z | |
| Stock to Leave | Radial and axial; negative values remove beyond the surface | 0 for a finish pass |
| Transition Type | Smooth or Straight between passes | Linking tab |
| Extend Before Retract | Extends the pass past the stock before retracting | Linking tab |
Tip: Face with a tool larger than the stock width if you can. A single pass produces a more consistent finish with no stepover marks. For a 50 mm wide bar, a 63 mm face mill takes one pass (general practice).
2D Contour#
Step by step#
- Milling > 2D > 2D Contour.
- Tool: choose a flat end mill with flute length at least the depth you cut.
- Geometry: select a face, edges or sketch curves. Selecting a face creates toolpaths on all its edges; use edge selection for areas with holes or pockets on the face. Contour arrows show the direction.
- Heights: Top = stock top; Bottom = the contour, with a negative offset if you need to cut cleanly through.
- Passes: set Sideways Compensation, Compensation Type, multiple depths and finishing passes.
- Linking: set the lead-in and lead-out.
- Click OK.
Compensation#
Passes tab > Compensation Type:
| Compensation type | Meaning |
|---|---|
| In computer | Fusion offsets the path by the tool diameter; the output has the compensated path, not G41/G42 |
| In control | No offset is calculated; G41/G42 codes are output so the operator sets compensation and wear at the control |
| Wear | Like In computer, but G41/G42 are also output so the operator can adjust for tool wear |
| Inverse wear | Identical to Wear, but the wear adjustment is entered as a positive number |
Control compensation (including Wear and Inverse wear) is applied only on finishing passes. Sideways Compensation chooses Left (climb milling) or Right (conventional milling). Compensation Radius Allowance sets a range of tool radii (from the selected radius up to radius plus the allowance) that can be used safely. Outer Corner Mode (shown when Compensation Type is In computer) offers Roll around corner, Keep sharp corner and Keep sharp corner with loop.
Tip: Compensation "in control" lets the operator measure a finished part and tweak the diameter offset without reposting. Check that your post supports it.
Stock to leave and finishing#
On the Passes tab:
- Stock to Leave: radial (wall) and axial (floor); negative values remove beyond the part surface.
- Multiple Depths with Maximum Stepdown.
- Multiple Finishing Passes: Number of Finishing Passes, Stepover, Finish Feedrate, Leads on all Finishing Passes.
- Repeat Finishing Pass repeats the final pass to remove stock left by deflection (a spring pass).
- Finishing Overlap, Lead End Distance, Finishing Smoothing Deviation, Preserve Order and Both Ways (for multiple depths on a single open contour).
- Tangential Extension Distance (and separate end extension) for open contours.
A common pattern (general practice): rough with 2D Adaptive Roughing leaving 0.3 mm radially, then finish with 2D Contour with a smaller tool at full depth with a spring pass.
Tabs#
On the Geometry tab, Tabs hold a workpiece while other material is machined away; Autodesk notes they are useful for thin plastic or wood on 2D routers. Options: Tab Shape (Rectangular or Triangular), Tab Width, Tab Height, Tab Positioning (By distance with Tab Distance, or Number of tabs per contour) and Manual Tabs (click on the contour). Alternatives: leave a floor of stock with a bottom offset, a vacuum table, or tape.
Lead-in and lead-out#
On the Linking tab:
- Lead-In (Entry): Horizontal Lead-In Radius, Lead-In Sweep Angle, Linear Lead-In Distance, Perpendicular, and Vertical Lead-In Radius.
- Lead-Out (Exit): Same as Lead-In, or separate horizontal radius, sweep angle, linear distance and vertical radius.
- Ramp: Ramping Angle, Maximum Ramp Stepdown, Ramp Clearance Height; Predrill Positions and Entry Positions are also offered.
- High Feedrate Mode, Allow Rapid Retract, Safe Distance, Keep Tool Down with Maximum Stay-Down Distance, and Lift Height control retracts.
For inside profiles, make sure the lead-in fits, or use a ramped entry to avoid gouging. Do not plunge a non-center-cutting end mill.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Tool / Preset | Selects tool and cutting data | Tool tab |
| Contour selection | Face, edge or sketch defining the contour | Geometry tab |
| Stock Contours | Considers stock or a selected boundary | Geometry tab |
| Compensation Type | In computer, In control, Wear, Inverse wear | Passes tab |
| Sideways Compensation | Left (climb) or Right (conventional) | Passes tab |
| Clearance / Retract / Feed / Top / Bottom height | Vertical limits | Heights tab |
| Multiple Depths | Splits the cut into Z steps | Set Maximum Stepdown |
| Stock to Leave (radial/axial) | Leaves material for later passes | Finishing default 0 |
| Tabs | Holds parts in place | Rectangular or triangular |
| Lead-In / Lead-Out | Approach and exit moves | Linking tab |
| Ramp | Entry moves into closed regions | Linking tab |
| Rest Machining | Removes only what a previous tool left | Tool diameter and corner radius |
Tips and pitfalls#
Tip: Chain selection can run into trouble where a sketch has tiny gaps or overlapping segments. If the chain stops early, clean the sketch (see the sketching section) or select edges of a solid face instead.
Tip: Cutting an outside profile through the stock? A small negative bottom offset (cutting into a spoilboard) is common practice, only if your fixture allows it. Otherwise add tabs or leave a skin.
Warning: If Top Height is lower than the stock top, the tool will plunge through uncut stock at rapid. Check the Heights tab visually: the preview shows the heights in the canvas.
Warning: Outside contour with climb direction and "in control" compensation relies on the post and control for G41/G42. If the post does not support it, you may see no compensation codes at all. Review the posted code.
Warning: Facing with a stepover of 100 percent of the diameter leaves ridges and wear. Fusion's default is 95% of the cutter diameter less the corner radius.
Practice exercise#
Model a 100 x 60 x 12 mm plate with a rounded-rectangle outer shape (10 mm corner radii) and a 40 x 20 mm rectangular internal window. Create a Setup with stock offsets of 2 mm on sides and top.
- Add a Face using a 16 mm end mill (or face mill). Confirm it removes 2 mm.
- Add a 2D Contour for the outer profile using a 10 mm flat end mill, Sideways Compensation Left (climb) on the outside, with four rectangular tabs of 5 mm width and 2 mm height.
- Add a 2D Contour for the internal window, climb direction on the inside, with a helical or ramp entry.
- Generate all three and Simulate.
Expected result: the simulation shows a faced top, a cut perimeter held by four small tabs, and a window with lead-in marks inside the material to be removed; there should be no gouges at the corners.
Related#
- Pocket and adaptive roughing
- Feeds and speeds
- Setups and stock
- Sketch best practices (Sketching section)