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Solid modeling environment

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    Procedures | References

    Base solids are imported models created in other CAD systems and saved as a native file or as a CAD neutral SAT or STEP file. You open a base solid in Autodesk Inventor as a fixed size base feature (the first one in a file). Unlike Autodesk Inventor models, you cannot access sketches or features used to create a base solid.

    There are two base solids editing environments in Inventor. If Inventor Fusion Technology is installed, editing a base solid launches Fusion and the base solid in edited in the Fusion environment. Once the Fusion editing session is ended and the Inventor environment is re-entered, the edited model is redisplayed in the Inventor graphics window showing any new or edited features.

    Editing base solids using Inventor Fusion Technology is the default setting. To disable this setting and use the normal Inventor base solids editing environment, click Application Options on the Tools tab. When the Application Options dialog box opens, click the Part tab and activate the Legacy Solid Edit environment option at the lower left of the dialog box.

    The other environment in which to edit base solids is the normal solids environment in Inventor when Inventor Fusion Technology is not installed. In the Inventor solids environment, you use commands to modify an imported base solid. Modifications do not add features to the solid, except for work features used as construction geometry . The remaining topics in this Help section refer to the normal Inventor base solids environment.

    How is the Inventor base solids environment different from the part environment?

     

     

    Part environment

    Solids environment

    File open

    Automatically in environment when you create or open a file.

    Double-click the base solid icon in the browser to activate the solids environment, or right-click over the base solid icon and select Edit Solid from the pop-up context menu.

    Commands

    Create and manipulate sketches and features, which combine to form parts.

    Feature and sketch commands add geometry to a base solid until the solids environment is activated.

    Specialized commands extend or contract a base solid and manipulate and delete faces .

    Geometry

    Relate geometric elements by dimensions and constraints. Activate sketches or features to change values.

    Modifications are not parametric and do not add features. Work features can be added as construction geometry. Use Update to close the solids environment.

    What tasks are performed in the solids environment?

    • Position work features for use as construction geometry.
    • Extend or contract a base solid about a work plane or planar face.
    • Move one or more faces nonparametrically.
    • Delete a base solid after retaining edges of a face for use as a profile .

    You can use the Measure and Precise Input commands to enter values when resizing a base solid.

    When you update the base solid to incorporate changes, features added in the part environment are repositioned.

    Which tasks are unavailable in the solids environment?

    You cannot add, modify, or delete these elements in the solids environment:

    • Dimensions
    • Constraints
    • Sketches
    • Features, except work features

    How do I edit a base solid using Inventor Fusion Technology?

    1. Start Inventor.
    2. Open a base solid (SAT or STEP file), and then double-click the base solid in the browser to launch Inventor Fusion Technology. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the pop-up context menu.
    3. A message box informs you that Fusion will be launched and that Inventor will be inaccessible. Click OK to close the dialog box and open Fusion.
    4. Edit existing features, or add new features to the model, in Inventor Fusion Technology.
    5. When you are finished, click the Return to Inventor command on the Fusion toolbar to save the edited model in .SAT format and return to the Inventor environment.
    TipUse the Fusion Save As command to save the model in a format other than .SAT before returning to Inventor.
    NoteRefer to the Help sections in Inventor Fusion Technology to learn more about creating and editing Fusion models.

     

    Procedures

    Move a face on a base solid or feature

     
    		 
    		 

    Use Move Face to move one or more faces on a feature or base solid. In parts, assemblies and weldments, moved faces are parametric, but they are not for solids.

    In the Solids environment, you usually select all faces that must move. Because faces are not parametrically associated, moving them as a group is the easiest way to retain their positions relative to one another.

    In the Part, Assembly, and Weldment environments, you can specify an explicit direction and distance to move a set of faces. You can also freely move and rotate a set of faces or features about the X, Y, or Z axes.

    		 

    Move faces using Free Move

    Open the file to edit:

    • Open a part, assembly, or weldment assembly document.
    • Open a base solid (specific non-native CAD file or a SAT or STEP file), and double-click the base solid in the browser to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the context menu.
    1. In a weldment, double-click the Preparations folder in the browser.
    2. On the ribbon, click Model tabModify panel Move Face.
    3. The Free Move option is active by default.
    4. Click one or more faces to move.
    5. Click the red, green, or blue triad to dynamically drag the face (or faces) along the X, Y, or Z axes, respectively. You can also enter a numeric value in the value input box.
    6. Click the OK button in the mini-toolbar to complete the operation and exit the command. Or, click the Apply button to implement the changes and select additional faces to apply cumulative linear or rotational transforms.

    In the Part, Assembly, and Weldment environments, a Move Face feature is added to the Model browser.

    Rotate faces using Free Move

    Open the file to edit:

    • Open a part, assembly, or weldment assembly document.
    • Open a base solid (specific non-native CAD file or a SAT or STEP file), and then double-click the base solid in the browser to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the context menu.
    1. In a weldment, double-click the Preparations folder in the browser.
    2. On the ribbon, click Model tabModify panel Move Face.
    3. The Free Move option is active by default.
    4. Click one or more faces to rotate.
    5. Click the red rotational manipulator to dynamically rotate in the YZ plane around the X axis. Click the green rotational manipulator to dynamically rotate in the XZ plane around the Y axis. Click the blue rotational manipulator to dynamically rotate in the XY plane around the Z axis. You can also enter an angular value in the value input box.
    6. Click the OK button in the mini-toolbar to complete the operation and exit the command. Or, click the Apply button to effect the changes and select additional faces to apply cumulative linear or rotational transforms.

    In the Part, Assembly, and Weldment environments, a Move Face feature is added to the Model browser.

    Reorienting the triad

    Open the file to edit:

    • Open a part, assembly, or weldment assembly document.
    • Open a base solid (specific non-native CAD file or a SAT or STEP file), and then double-click the base solid in the browser to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the context menu.
    1. In a weldment, double-click the Preparations folder in the browser.
    2. On the ribbon, click Model tabModify panel Move Face.
    3. The Free Move option is active by default.
    4. Click one or more faces to move or rotate.
    5. Click the triad linear, rotational, or planar axis to be reoriented.
    6. Click the Triad Reorientation button in the mini-toolbar.
    7. Select a linear edge or planar face to reorient the triad. Work planes, work axes, 2D and 3D sketch curves are also valid selections for triad reorientation.
    8. When the triad is reoriented to your satisfaction, proceed with the Free Move operation.

    In the Part, Assembly, and Weldment environments, a Move Face feature is added to the browser.

    Snapping to a face or work point

    You can move or rotate a face to align with another face or work point using the Snap To button on the mini-toolbar. Only a single face can be moved or rotated at one time.

    Open the file to edit:

    • Open a part, assembly, or weldment assembly document.
    • Open a base solid (specific non-native CAD file or a SAT or STEP file), and then double-click the base solid in the browser to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the context menu.
    1. In a weldment, double-click the Preparations folder in the browser.
    2. On the ribbon, click Model tabModify panel Move Face.
    3. The Free Move option is active by default.
    4. Select the face to be realigned.
    5. Click the triad linear axis or rotational manipulator that matches the orientation of the face you wish to snap to. If a linear or planar move is selected on the triad, then the face will move to alignment. If rotation is selected, then the face will rotate to alignment.
    6. Click the Snap To button in the mini-toolbar.
    7. Select the face or work point to align with.

    In the Part, Assembly, and Weldment environments, a Move Face feature is added to the Model browser.

    Move faces by direction and distance

    Open the file to edit:

    • Open a part, assembly, or weldment assembly document.
    • Open a base solid (specific non-native CAD file or a SAT or STEP file), and then double-click the base solid in the browser to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the context menu.
    1. In a weldment, double-click the Preparations folder in the browser.
    2. On the ribbon, click Model tabModify panel Move Face.
    3. Click one or more faces to move.
    4. Click Direction and Distance.
    5. In the graphics window, click a face, an edge, or work axis to define the direction. The default direction is the reverse direction of normal for a selected face. You can click Flip to reverse direction.
    6. Enter the distance one of these ways:
      • Enter a number or an equation. The equation cannot include a parameter name.
      • Click the arrow to list recent values, and click a value to select it.
      • Click the arrow to access the Measure command. The measured value is automatically entered in the distance field.
    7. If editing a solid, click Update to close the Solids environment.

    In the Part, Assembly, and Weldment environments, a Move Face feature is added to the Model browser.

    Move a face by a distance in a plane

    Open the file to edit:

    • Open a part or assembly document.
    • Open a base solid (SAT or STEP file), and then double-click the base solid in the browser to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the context menu.
    1. In a weldment, double-click the Preparations folder in the browser.
    2. On the ribbon, click Model tabModify panel Move Face.
    3. Click one or more faces to move.
    4. Click Points and Plane.
    5. In the graphics window, click a plane.
    6. Click Points, and then click two points to define the start and endpoint.

      The points are projected onto the plane, if necessary, and one or more faces are moved relative to the projected points.

    7. If editing a base solid, click Update to close the Solids environment.

    Only work points, the endpoint or midpoint of a linear edge, or the center of a circular edge can be selected.

    In the Part, Assembly, and Weldment environments, a Move Face feature is added to the Model browser.

    Delete a base solid face or body

    In the solids environment, you can delete one or more faces from a base solid . Usually, you select all faces to delete as a group because dependent faces (for example, fillets) are not selected automatically.

    You can add sketched features to the base solid, delete the base solid, and then do one of the following:

    • Delete the sketches of dependent features .
    • Retain the sketches of dependent features.
    • Retain selected dependent features and sketches.

    To delete faces from a base solid

    Open a base solid (specific non-native CAD file or a SAT or STEP file), and then double-click the base solid in the browser to activate the Solids environment.

    1. Select one or more faces to delete.
    2. Right-click and select Delete.
    3. Click Update to close the Solids environment.

    To delete a base solid

    Open a base solid (SAT or STEP file). Create sketches to project boundaries automatically of the base solid onto the sketch plane , and use sketch commands to add new geometry as desired.

    After you add sketch geometry and sketched features to a base solid, you can delete the solid, but retain dependent features and sketches.

    1. Double-click the base solid in the browser to activate the Solids environment.
    2. Select the base solid in the graphics window or in the browser, and then right-click and select Delete.
    3. If the base solid has dependent sketched features, do one of the following:
      • Click OK to delete features and their consumed sketches.
      • Select check boxes to retain the dependent features, retain the consumed sketches, or both, then click OK.
    4. Click Update to close the Solids environment.

    You can constrain the sketches to work planes or use Reattach Sketch to move sketches onto other work planes.

     

    Extend or contract a base solid

     
    		 
    		 

    Use Extend or Contract Body in the solids environment to lengthen or shorten a base solid symmetrically about a planar face or work plane .

    To begin, open a base solid (SAT or STEP file). If desired, position a work plane at the point where you want to extend or contract the base solid .

     
    1. On the ribbon, click Edit Base Solid tabModify panel Extend/Contract Body.
    2. Click Plane, then select the work plane or planar face.
    3. Click Extend or Contract.
    4. Enter the distance to extend or contract or click the arrow to list and select recent values.

      If desired, you can express the distance as an equation.

    5. Click Update to close the solids environment.
    NoteIf you prefer, you can select a planar face as the section plane.

    References

    Move faces

     
    		 

    Moves one or more faces on a base solid or a feature by a specified distance and direction or by a planar move to specific coordinates.

    In the part or assembly environment, moved faces are parametric. In the solids environment, moved faces are not parametric. In weldments, use Move Face to move a face to leave welding clearance.

    Access:

    In the Part or assembly environment, click Model tab Modify panel Move Face. In weldment assemblies, double-click the Preparations folder in the browser and then click Weld tab Preparation and Machining panel Move Face

    Right-click the component in the browser and select Edit Solid to activate the Solids environment. Alternatively, you can right-click over the base solid in the browser and select Edit Solid from the pop-up context menu. Then click Edit Base Solid tab Modify panel Move Face.

    Faces

    Selects one or more faces to move.

    Automatic Blending

    Automatic blending is a re-blending technology that automatically moves adjacent tangential faces and also creates new blends, if required. It is active by default in the part modeling, assembly, and solid edit environments.

    The Automatic Blending check box is active for both the Direction and Distance and Points and Plane options for new models. However, the check box is deactivated for models created prior to Inventor 2011 (legacy models).

    Features created using the default Free Move option always use automatic blending, so the check box is not displayed when Free Move is active.

    Free Move

     

    Free Move is a non-parametric move type that allows cumulative linear and rotational transforms of faces using a 3D in-canvas tool called the Triad. You can interactively position a face or feature by dragging the triad in a planar move, axial move, or free movement. The selected area of the triad controls the movement

    .
     

    When the triad is displayed, select or drag a triad segment to indicate the type of transform you want. You can enter coordinates to move a face or feature precisely using the value input box. When you drag or rotate the triad, the X, Y, and Z coordinates or angular values dynamically update in the value input box.

     

    The colors help you identify the triad axes:

    • Red is the X axis
    • Green is the Y axis
    • Blue is the Z axis

    When you first activate the triad, its origin sphere is coincident with the geometry you want to transform. Click a triad section or drag to indicate the type of transform you want. As you select other parts of the triad, you can drag or enter precise coordinates corresponding to your selection.

    Triad Part

    Description

    Arrowheads

    Moves the triad along the axis.

    Rotational manipulators

    Rotates the triad around the axis.

    Planes

    Moves the triad in the selected plane.

    Sphere

    Allows unrestricted movement in the view plane.

    Reorienting the Triad

     

    Triad Reorientation Whether selecting one or multiple faces, the initial alignment of the Free Move triad depends on the first selected face. In many cases, the triad alignment may be satisfactory for the operation you wish to perform. If not, use the Triad Reorientation button in the mini-toolbar to reorient the triad with a different face or feature. Permissible selections include: any face or edge geometry, vertices, work planes, work axes, work points, sketch curves, 2D and 3D points.

    Snapping to a face or work point

     

    Snap To in the mini-toolbar moves a face to align with another face, plane, vertex, or work point. Selected faces may be cylindrical or planar, and planar faces may be at different angles. Only a single face may be moved or rotated at a time.

    Direction and Distance

     

    Direction and Distance moves faces in a specified direction and distance. The direction defaults to the reverse normal for the selected face.

     

     

    Direction selects the edge or work axis to define direction.

     

     

    Distance sets the distance faces move. May be expressed as an equation or a recent value selected from list. If desired, select Measure to use the measure command or Show Dimensions.

    Points and Plane

     

    Points and Plane moves faces between selected points on a plane.

     

     

    Plane selects the plane on which faces move.

     

     

    Points sets the beginning and ending points to specify move of faces. Draws a temporary line to show the vector.

    Extend or contract body

     
    		 
    		 

    In the solids environment, extends or contracts a base solid along an axis. The base solid is resized perpendicular to a selected plane. Extending or contracting a base solid does not add a new feature.

    Access:

    Right-click the component in the browser, and select Edit Solid to activate the solids environment. Then click Edit Base Solid tab Modify panel Extend/Contract Body.

    Plane

    Selects a work plane or planar face to identify the section about which the base solid extends or contracts.

    Extend or Contract

     

    Specifies if the base solid extends or contracts equally on both sides of the selected plane by a specified distance.

    Distance

    Specifies distance the base solid extends or contracts. May be specified as a number or an equation.

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