Additional Surface Tools

Transcription

1 Additional Surface Tools Several additional surface tools, techniques, and related functions are available. This supplement provides a brief introduction to those functions. Panel Part Features Replace Face Replacing Faces The shape of an existing feature face can be replaced using a surface, quilt, solid, or work plane. Replace faces to develop or finalize a model or to explore design alternatives or product changes without having to remove or further edit original features. The surface or quilt used to replace an existing face must be the same size as, or larger than, the existing face. See Figure 13A-1A. This requirement is common for creating or modifying solids using surfaces. If the shape is not large enough, as shown in Figure 13A-1B, or if faces are perpendicular to the new shape, the new face will not form. Replace faces using the Replace Face tool and Replace Face dialog box. See Figure 13A-2. The Select Existing Faces button is active by default, allowing you to choose existing feature faces to replace. Next, pick the Select New Faces button and pick one or more surfaces or quilts to define the shape of the new feature face. If the faces you select contain multiple tangent faces, pick the Automatic Face Chain check box in order to select all the faces, instead of having to select each face individually. Finally, pick the OK button to generate the new face. Inventor

2 Figure 13A 1 A An example of exploring an alternative design by replacing a feature face. This example shows a replaced face removing material. A replaced face can also add material to a model by filling the space between the original face and new face. B The new face reference must completely cover the original face. Surface added to replace existing face Replaced face (surface visible for reference) Surface not large enough to replace face Existing Feature face A B Figure 13A 2 The Replace Face dialog box. Pick to select multiple tangent faces When AutoCAD is configured to display a screen menu, the commands appear in a separate screen. NOTE Replaced faces are not consumed by the feature, which still contains the original face, as evident by the separate Replace Face item in the browser. Inventor

3 Panel Part Features Sculpt Sculpting In order to sculpt a solid, first create the intersecting surfaces that define the size and shape, or boundaries, of the solid. See Figure 13A-3A. Then, use the Sculpt tool and Sculpt dialog box to create the sculpted feature. See Figure 13A-3B. Select the Add button to add Figure 13A 3 A An example of surfaces forming sculpt boundaries. B Using the Sculpt dialog box to select surfaces and define parameters. C A sculpted solid. Work plane Surface loft Surface extrusion Pick to add material Pick to remove material Preview Pick an arrow or the sphere to define the sculpt direction A Use instead of flip arrows in model to refine the direction B C Inventor

4 material to the model during the sculpt operation, or pick the Remove button to remove material. The Remove button is disabled if no solids are present in the model. The Surfaces button is selected, allowing you to choose the surfaces to form the feature. A preview appears if appropriate boundaries are found. The direction arrows that appear in the model allow you to define the direction from the surfaces used to produce the feature. The arrows should point toward the area where the solid will form. Pick the sphere to specify both directions. Direction can also be set by picking the More button in the Sculpt dialog box and selecting the appropriate direction from the flyout corresponding to the surface listed in the Side Selection list. When you have specified all of the sculpt options, pick the OK button to generate the solid. See Figure 13A-3C. Figure 13A-4 shows an example of a sculpt created using the remove operation. The remove operation does not require a surface on all sides of the removed area. In Figure 13A-4B, the incorrect side from the work plane is designated to be removed. To solve this problem, pick the direction arrow in the model or use the Sculpt dialog box. See Figure 13A-4C. PROFESSIONAL TIP An unnecessary surface selection can cause an error when sculpting. Delete a selection from the Side Selection list by picking the surface and pressing [Delete]. Inventor

5 Figure 13A 4 A An example of surfaces that can be used to remove material during a sculpt operation. Extruded surface Work plane A Inventor

6 Figure 13A 4 (continued) B Using the Sculpt dialog box to remove the solid between boundaries. Preview B Inventor

7 Figure 13A 4 (continued) C Redefining the side to sculpt. D The completed sculpt. Flipped direction New preview Flipped direction C D Inventor

8 Deleting Faces, Lumps, and Voids Often, especially when you are developing complex feature geometry, unnecessary faces, lumps, and voids appear. In certain situations, deleting a face, lump, or void is useful and may even be required. These items should be removed as necessary to create a clean model and to ensure that mass properties are calculated correctly. Panel Part Features Delete Face Deleting Faces Use the Delete Face tool and Delete dialog box to remove faces, lumps, and voids. By default, the Select Individual Faces button is selected, which is used to select one or more faces for deletion. Use the Activate Faces button to pick the faces to remove. Figure 13A-5A shows an example of multiple faces left over from a cut sweep operation. When deleting faces, be sure you select all of the faces to remove. To create the final model shown in Figure 13A-5B, six faces are removed. Inventor

9 Figure 13A 5 A Unwanted faces left during a cut-sweep operation selected for deletion. B Faces removed. Pick to remove faces A B Inventor

10 Another application for deleting a face is to remove all volume from a feature or part, transforming the model into a surface. Apply this technique when you want to use an existing solid to generate a surface or quilt for additional modeling purposes. An example is creating a volumeless surface copy of a part for establishing decals. The surface icon replaces the part icon, and the deleted face operation appears in the browser. See Figure 13A-6. Figure 13A 6 An example of using the Delete Face tool to create a surface model. Original Solid Model Surface icon Bottom face deleted New Surface Model (rotated for clarity) Inventor

11 To delete a face and repair the gap that is created by removing the face, select the Heal check box in the Delete Face dialog box. When a deleted face is healed, the faces that are adjacent to the removal come together. Heal deleted faces when you want to remove a specific face without completely removing or editing a feature. Figure 13A-7 shows an example of the healing concept. CAUTION Use caution when deleting faces. Be sure the faces you remove do not make the model a loose mass, unless this is the desired effect. Figure 13A 7 An example of the effects of deleting and healing a face. Original selected face Face healed Inventor

12 Deleting Lumps and Voids A lump can be as simple as a single extrusion, or as complex as a multi-feature part. In some situations, multiple lumps are created in a single part, and you may want to delete one or more of these lumps. For example, two lumps are created when you extrude a sketch of two individual circles. Later in the design process, you may want to delete one of the lump cylinders. To delete a lump, pick the Select lump or void button in the Delete Face dialog box, and select one or more lumps to delete. See Figure 13A-8. Figure 13A 8 A Selecting a lump to delete. B The part after the lump is removed. Pick to delete a lump Selected lump A B Inventor

13 A void may occur during certain modeling operations. For example, if you extrude a sketch of two rectangles and then shell one of the extrusions, the shell actually creates a void in both extrusions even though you only selected one face to remove. See Figure 13A-9. In some situations, a void may not be a problem, but voids do affect the mass properties of a solid and complicate the development of additional features that might intersect the void. To delete a void, pick the Select lump or void button and select one or more voids to delete. Voids are inside of model geometry, so in order to select and delete a void, you must cycle through possible selections using the Select Other tool or the wheel on the mouse. Figure 13A 9 Deleting a void. Shell removes selected face only Void Use to help select a void Pick to delete a void Inventor

14 When AutoCAD is configured to display a screen menu, the commands appear in a separate screen. NOTE Do not confuse the process of deleting a face, lump, or void using the Delete Face tool with the process of removing a model item by picking the object and pressing the [Delete] key, or by right-clicking on an item and selecting Delete. These deleting options are very different and do not allow you to remove faces, lumps, or voids. Panel Part Features Boundary Patch Creating Boundary Patches Another method to create a construction surface is to form a boundary patch. A boundary patch is effective when you want to generate a planar surface using existing sketch geometry or feature edges. Use the Boundary Patch tool and Boundary Patch dialog box to create a boundary patch. Any unconsumed 2D sketch geometry can be used to form a construction surface. For example, the sketch shown in Figure 13A-10 was used to create the surface. If only one sketch profile is available, the sketch is automatically selected. If more than one sketch profile is present, individually pick the profiles to include in the boundary patch. Select the OK button to create the surface. Existing feature edges can also be used to create a construction surface. A continuous edge chain can be selected if available, but in most cases, you must pick individual edges to define a closed edge loop. See Figure 13A-11. An example of creating a boundary patch using the edge of Inventor

15 Figure 13A 10 Using a sketch profile to create a boundary patch. Selecting a Sketch Profile Boundary Patch Figure 13A 11 Forming a boundary patch between existing feature edges. First, select an edge Boundary patch Second, select the automatic edge chain Inventor

16 an existing surface is shown in Figure 13A-12. In this example, because the boundary path is adjacent to tangent surfaces, you have the option of applying a Free Condition or Tangent Condition to the feature. Pick the OK button to create the boundary patch. Figure 13A 12 A A surface revolution requiring a boundary patch. B Defining the boundary path parameters. Choose a free or tangent edge condition Surface revolution Selected edge A B Inventor

17 Figure 13A 12 (continued) C The boundary patch with a free condition. D The boundary patch with a tangent condition. Flat surface Curved surface Free Condition C Tangent Condition D Inventor

18 When AutoCAD is configured to display a screen menu, the commands appear in a separate screen. NOTE A construction surface created using the Boundary Patch tool is identified appropriately in the browser and consumes the selected sketch geometry. Panel Part Features Trim Surface Trimming and Extending Surfaces Surfaces are trimmed or extended to remove unnecessary surface information or create additional material to help create other surface features. To perform these tasks, use the Trim Surface and Extend Surface tools. Trimming Surfaces In order to trim a surface, you must have a cutting tool available to select. Then, access the Trim Surface tool to display the Trim Surface dialog box. See Figure 13A-13. The cutting tool may be selected automatically. If not, pick the Cutting Tool button and choose the cutting tool. Then select the side of the surface to trim using the active Remove button. If you select the incorrect side, pick the Invert Selection button to reverse the operation. Pick the OK button to trim the surface. Inventor

19 Figure 13A 13 Trimming a surface using the Trim Surface tool. Cutting tool Original Surface Pick to flip the side to remove Selected Portion to Remove Trimmed Surface Inventor

20 Panel Part Features Extend Surface Extending Surfaces Use the Extend Surface tool and Extend Surface dialog box to extend surfaces. See Figure 13A-14. Pick the Edges button if it is not already selected, and choose the surface edges to lengthen. Multiple tangent edges can be selected automatically by picking the Edge Chain check box. Then specify the length of the extension by selecting Distance or To from the Extents drop-down list. Use the Distance extent option to extend the edge to a desired length by entering a distance in the text box. See Figure 13A-14A. To terminate the edge at an existing surface or plane, pick the To extent option. Then pick the face or plane to which to extend the surface. See Figure 13A-14B. You may need to choose the Select surface to end the feature creation button if it is not already activated. If the face or plane you choose does not intersect the extrusion path, check the Terminate feature on the extended face check box. PROFESSIONAL TIP The Extend Surface tool is effective for extending surfaces used to produce split features and all other features that require a surface of a specific size. Inventor

21 Figure 13A 14 A Using the Distance option of the Extend Surface tool to extend the edge of a surface a specified distance. B Using the To option to extend the edge of a surface to another surface..5 extension preview Selected surface edge Use to adjust the edge extension according to the shape of adjacent edges A Selected surface edge Existing surface (opaque for clarity) Existing surface (opaque for clarity) Extension preview Selected termination plane B Inventor

22 Panel Part Features Stitch Surface Stitching Surfaces Individual surfaces can be stitched in order to eliminate separate surfaces that may cause modeling errors. Figure 13A-15 shows an example two surfaces side by side. One surface is opaque for clarity. Use the Stitch Surface tool and Stitch Surface dialog box to stitch these surfaces together. The Surfaces button is active by default, allowing you to select the surfaces to stitch. Pick the OK button to complete the operation. Figure 13A 15 Using the Stitch Surface dialog box to stitch surfaces. Separate surface (opaque for clarity) Separate surface Surfaces Requiring Stitching Stitched Quilt Inventor

23 Toolbar Inventor Standard Open Menu Browser File > Open Type [Ctrl]+[O] Menu Browser Insert > Import Stitching and Promoting Surfaces Surfaces can be imported into Inventor using the Open or Import tool. When you import surfaces into Inventor, the surfaces are placed in a nonparametric construction environment. This occurs because data used to create surfaces in.iges and.sat files, for example, are inconsistent with the data required by Inventor. Once imported, the surfaces may need to be stitched and promoted in order for the geometry to be useful in a model. PROFESSIONAL TIP You may be able to bypass the entire process of stitching and promoting surfaces by selecting the Auto Stitch and Promote check box of the Import Options dialog box. The Import Options dialog box is available by picking the Options... button in the Import and Open dialog boxes. Inventor