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Construction surfaces provide ways to describe shapes when creating extruded, revolved, swept, and lofted parts. For each of these features, you can choose to create a surface instead of a cut, join, or intersection.
You can use an open or closed profile to create a surface. The surface can then be used as a termination face for other features or used as a split tool to create a multi-body part.
Surfaces are not consumed by features.
A surface is represented in the browser as a suffix to the feature command used to create it (for example, ExtrusionSrf1, SweepSrf1, and so on).
How is the appearance and visibility of surfaces controlled?
You can change the appearance of a surface from translucent to opaque in the Application Options dialog box. On the Part tab, in the Construction category, select the Opaque Surfaces option. When you create a surface, it is opaque and is the same color as a work feature.
Surfaces created before the option is set are translucent. To change surface appearance, right-click the surface in the browser, and then select Translucent. Select or clear the check mark to switch opacity on and off.
In the graphics window, a surface is translucent by default, similar to a work plane. You can right-click a surface in the browser or graphics window, and then turn off its visibility.
Can surface shapes be modified?
If desired, you can use Fillet and Chamfer commands to modify sharp edges of surfaces.
You can also edit the profile shape. Expand the surface in the browser, right-click the sketch icon, and then select Edit Sketch.
In the part environment, you can use the Stitch command to stitch several edge-matched surfaces together to create a quilt. Unlike the Stitch command in the construction environment, this operation is parametric; changes to the parent surfaces update the quilted surface.
Which shapes are possible for surfaces created with different feature commands?
Examples of surfaces are shown clockwise from the top left corner:
- A revolved surface created from a sketched line rotated around an axis.
- A lofted surface created from two closed profiles.
- Extruded surfaces created from line segments extruded a specific distance. One uses fillets to round corners.
- A swept surface created by a profile containing lines and arcs swept along an arc.
- A revolved surface created by a spline rotated around an axis.
Create a construction surface
The Surface operation is available for the Revolve, Loft, Extrude, Sweep, and Thicken commands on the 3D Model tab. Specific requirements for creating a surface depend on the feature command you use.
A construction surface is created from an open or closed profile. Use the Thicken command to create a construction surface offsetting one or more surfaces.
Use a surface as a termination plane to refine shapes or as a split tool when creating a multi-body part. After you use the surface as a termination plane or a split tool, you can turn off its visibility.
Like the planar face of a solid model, a construction surface can be used as a sketch plane.
To create opaque surfaces, select
Options to access the Application Options dialog box and then click the Part tab. Under Construction, select the Opaque Surfaces option. If you prefer, change surface appearance after you create them. Right-click individual surfaces in the browser, and then select Translucent. To change a surface appearance, right-click a surface and choose Properties. Change the Feature Appearance to what is appropriate.
- On the ribbon, click and select a face or work plane as the sketch plane.
- Use command on the Sketch tab to create an open or closed profile to represent the shape.
- Create other geometry as required by the command used to create the surface (such as an axis or second profile for a loft).
- On the 3D Model tab, Create panel, click the Extrude, Revolve, Loft, or Sweep command.
- When a profile is detected, the Surface operation is automatically selected. Select other geometry as required by the command.
- If desired, enter additional values to define the surface for the command (such as a taper angle and distance, revolution angle, or point mapping, if available).
- Click OK.
Create one or more features, selecting the construction surface when a termination plane is required or as the cutting line to split a part. If desired, you can use multiple construction surfaces as the beginning and ending termination planes.
Stitch surfaces together in the Part environment
You can stitch surfaces together into a quilt. To stitch successfully, edges must be exactly the same size and adjacent to each other.
Use Stitch in the part environment to combine surfaces whose edges are exactly the same size. A stitch feature is placed in the browser.
- On the ribbon, click . The Stitch dialog box is displayed.
- Choose a method to select surfaces:
- Right-click and choose Select All from the context menu to select all surfaces at once.
- In the graphics window, click to select one or more individual surfaces. As the surfaces are selected, the edge conditions are displayed. Edges without a co-edge become red in color. Successfully stitched edges are black.
- Click the Analyze tab to enable/disable edge analysis and assess edges before stitching together.
NoteChecking tangent edge analysis decreases system performance.
- Click the Stitch tab.
- Set the tolerance.
- If appropriate, enable the Maintain as surface check box.
- Click Apply to join surfaces together in a quilt or solid.
- All newly stitched edges are now black. The remaining free edges are still red and are listed in the Find Remaining Free Edges list with the maximum distance each edge pair is from the other. Free edges that are not selected and considered for stitching has no value.
- To stitch surfaces that were unsuccessful the first time, use tolerance control by selecting or entering a value in the Maximum Tolerance list. Look at the remaining edge pairs that you want to stitch together and the smallest associated Max Gap value. The Max Gap value is the largest gap that the Stitch command considers for making a tolerant edge. Use the smallest Max Gap value as a guide for entering a Maximum Tolerance value. For example, a Max Gap of 0.00362 must have a value of 0.004 entered in the Maximum Tolerance list to enable a successful stitch.
Note You can right-click a value in the list to use as the Maximum Tolerance value.
- Click Apply. All newly stitched edges are now black.
- When stitching is complete, click Done. All edges return to their original color before entering the Stitch command.
NoteBy default, stitch features consume input surface features such as extruded or revolved surfaces. Consumed features are nested and indented below the consumer to show the dependency on that feature. In cases where consumption is not desirable, you can right-click in the browser, and then select Consume Inputs to change the consumption status.
Stitch surfaces (Part environment)
Stitches surfaces together to form a quilt or solid. Surface edges must be adjacent to stitch successfully. The stitch command has a tolerance control that provides an upper limit and helps Autodesk Inventor determine the proper edges to be used for stitching.
Selects parametric surfaces to stitch together into a quilt or solid body. Also used to analyze whether surfaces are suitable for stitching. Creates a stitch feature that can be edited later.
Surfaces. Selects individual or all surfaces to stitch together into a quilt or analyze. Surfaces are highlighted in the graphics window as they are selected.
Maximum Tolerance. Select or enter a value for the maximum allowable tolerance between free edges.
Find Remaining Free Edges. Displays the free edges that remain after stitching and the maximum gap between them.
- Select a row item and right-click on it to display the context menu.
- Select Find in Window, to zoom in on the edge.
- Select Set as Tolerance, to quickly change the maximum tolerance used in stitching.
- Free edge pairs display the value of the maximum gap between them.
- Free edge pairs which partially exceed the maximum tolerance, display the minimum gap in Red (meaning that the gap is within tolerance but not fixed).
- Free edges without pairs display no gap value.
Maintain as surface. If not selected, a stitched surface with a valid closed volume is solidified. If selected, the stitched surface remains a surface.
Analyzes selected surfaces and marks surface edges with condition to indicate suitability for stitching into a quilt. Identifies surfaces that have gaps or tolerance errors.
Show Edge Conditions. When checked, this option identifies surface edges by color to show results of analysis.
- Black edges are stitched to an adjacent surface.
- Red edges are free edges on a surface, and are not stitched to an adjacent surface.
Show Near Tangent. When checked, this option shows near tangent conditions.
- Magenta edges have some discontinuity to the adjacent surface (are nearly tangent). These edges can cause failures in subsequent design operations such as creating a shell.
NoteThis option has an impact on performance.
Maintain as surface
Select to maintain closed volume as surfaces. If not selected, a closed volume that results from the stitch operation becomes a solid.
Stitches selected surfaces into a quilt.