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Work planes

    Procedures | References
     

    Work features are abstract construction geometry used when geometry is insufficient for creating and positioning new features. To fix position and shape, constrain features to work features.

    Use work planes when creating axes, sketch planes, or termination planes, or to position cross-sectional views or cutting planes.

    Use a work plane when:

    • A part face is not available as a sketch plane for sketching new features.
    • An intermediate position is required to define other work planes (for example, at an angle to a face at an offset distance).

    Place work planes at the center of cylindrical shapes and use them to anchor parametric dimensions between cylindrical features.

    When creating 3D features, place a work point at the intersection of work axes and work planes. You select the work points to specify the path of the sweep.

     

    Procedures

    Create a work plane

     

    On the ribbon, use the Model tab Work Features panel Plane command to define a work plane using feature vertices , edges , faces , or other work features. Except in an assembly, you can create in-line work planes when a work feature command requires you to select a plane.

    In an assembly , use the Plane command on the Model tab to define work planes that reside in the assembly, not in a part model. You can create a work plane mid-way between planar faces on a single part while editing the part. Midpoints are not selectable in an assembly.

    Prior to the introduction of Direct Manipulation modeling techniques in Inventor R2011, the Plane command was the only method available to create work planes. This legacy method was, and still can be, used with one or more of the following relationships to define a work plane:

    • On geometry (on three points, for example)
    • Normal to geometry
    • Parallel to geometry
    • At an angle to geometry (on a plane and an axis)
    TipTo understand geometric dependencies, right-click a work feature in the browser or the graphics window, and then select Show Inputs. For example, you can right-click a work point to highlight the geometry from which it was created, such as a work axis and a work plane.
    NoteAlthough still valid, the Plane command has been enhanced in Inventor R2011 to now present the Inventor user with a convenient drop-down menu listing each of the possible combinations available for work plane creation. Each of these new options is described on the Quick Reference tab of this Help topic.
     
    1. On the ribbon, click Model tabWork Features panel Plane.
    2. Select appropriate vertices, edges, or faces to define a work plane.
    3. For offset work planes, drag the work plane to the appropriate location and enter a distance or angle in the Offset edit box. Click the check mark in the edit box to accept the preview and create the offset work plane.

      If more than one solution is possible, a selection box appears. Click the forward or reverse arrows in the selection box, and then click the check mark when the correct solution is previewed.

    4. Optionally, resize the work plane. Right-click the work plane and clear the check mark from Auto-Resize, if necessary. Click a grip handle on one of the work plane corners and drag to resize.

    Show Me how to create a work plane normal to an edge through a point

     

    Show Me how to create a work plane parallel to a face through a point

     

    Show Me how to use sketch geometry to create a work plane

     

    Show Me how to create a work plane tangent to a circular face and parallel to a face

     

    Show Me how to create a three-point work plane

     

    Show Me how to create a two-edge or two-axis work plane

     

    Show Me how to create a workplane perpendicular to a curve

     

    Show Me how to create a work plane tangent to a circular face and through an edge

     

    NoteIf appropriate, you can create work planes offset from one another at a specific distance or angle. Follow the previous steps, selecting the last created work plane, and then drag the new work plane to the offset distance.

    Create work planes through axes and at angles to existing planes

    1. In an assembly file, click Model tabWork Features panel Plane
    2. Select a PLANE and a LINE.
      NoteThe selection order does not matter. The PLANE and LINE must be parallel to each other.

      The PLANE can be a:

      • Planar face in the graphics window
      • Work plane in the graphics window or browser
      • Sketch in browser

      The LINE can be a:

      • Linear edge in the graphics window
      • Work axis in the graphics window or browser
      • 2D sketch line in the graphics window
      • 3D sketch line in the graphics window
    3. Enter an angle in the Angle dialog box. As you change the angle, the preview updates automatically.
    4. Click the check mark in the Angle dialog box or press Enter.

     

    Resize or move a work plane

     

    Drag a corner or edge of a work plane to resize or move it.

     
    1. On the ribbon, click Model tabWork Features panel Plane. Select appropriate vertices, edges, or faces to define a work plane, or select the desired option from the Plane drop-down menu.
    2. Adjust the size and position of the work plane:
      • Click a corner to display the Resize symbol. Drag the corner to the appropriate size and release.
      • Click an edge to display the Move symbol. Drag the edge to the appropriate position and release.

    Show Me how to resize work planes in an assembly document

     

     

    References

    Work planes

     

    In a part, a work plane is an infinite construction plane that is parametrically attached to a feature. In an assembly, a work plane is constrained relative to an existing component.

    Work planes can be placed at any orientation in space, offset from existing faces, or rotated around an axis or edge. A work plane can be used as a sketch plane and dimensioned or constrained to other features or components. In an assembly, you can create a work plane between two planar faces on separate components.

    Each work plane has its own internal coordinate system. The order in which geometry is selected determines the origin and positive directions of the coordinate system axes.

    In a part, a work plane can be created in-line while you are using another work feature command. The Work Plane command terminates as soon as the work plane is created.

    NoteOptionally, you can resize a work plane. Right-click a work plane and clear the check mark from Auto-Resize, if necessary. Click a grip handle on one of the workplane corners and drag to resize.

    Access:

    		Ribbon: Model tab Work Features panel Plane
    TipTo understand geometric dependencies, right-click a work feature in the browser or the graphics window, and then select Show Inputs. For example, you can right-click a work point to highlight the geometry from which it was created, such as a work axis and a work plane.

    The Plane drop-down menu offers the following work plane creation options:

     

    Plane (legacy method)

    Select:

    Appropriate vertices, edges, or faces to define a work plane

    Result:

    Creates a work plane through the selected objects.

     

    Offset from Plane

    Select:

    A planar face. Click the face and drag in the direction of the offset. Enter a value in the edit box to specify the offset distance.

    Result:

    Creates a work plane parallel to the selected face at the specified offset distance.

     

    Parallel to Plane through Point

    Select:

    A planar face or work plane and any point, in either order.

    Result:

    The work plane coordinate system is derived from the plane selected.

     

    Midplane between Two Parallel Planes

    Select:

    		Two parallel planar faces or work planes.

    Result:

    The new work plane is oriented to the coordinate system and has the same outward normal of the first selected plane.

     

    Midplane of Torus

    Select:

    A torus.

    Result:

    		The work plane is created through the center, or midplane, of the torus.
     

    Angle to Plane around Edge

    Select:

    A part face or plane and any edge or line parallel to the face.

    Result:

    Creates a work plane angled 90 degrees from the part face or plane. Enter the desired angle in the edit box and click the check mark to reset at the new angle.

     

    Three Points

    Select:

    Any three points (endpoints, intersections, midpoints, work points).

    Result:

    The positive X axis is directed from the first point to the second point. The positive Y axis is perpendicular to the positive X axis through the third point.

     

    Two Coplanar Edges

    Select:

    Two coplanar work axes, edges, or lines.

    Result:

    The positive X axis is oriented along the first selected edge.

     

    Tangent to Surface through Edge

    Select:

    A curved face and a linear edge, in either order.

    Result:

    The X axis is defined by the line of tangency to the face. The positive Y axis is defined from the X axis to the edge.

     

    Tangent to Surface through Point

    Select:

    A curved face and an endpoint, midpoint, or work point.

    Result:

    The X axis is defined by the line of tangency to the face. The positive Y axis is defined from the X axis to the point.

     

    Tangent to Surface and Parallel to Plane

    Select:

    		A curved face and a planar face or work plane, in either order.

    Result:

    The new work plane coordinate system is derived from the selected plane. This method can also be used to create a work plane tangent to a face or plane that is normal to a plane.

     

    Normal to Axis through Point

    Select:

    		A linear edge or axis and a point, in either order.

    Result:

    		The positive X axis is oriented from the intersection of the plane and axis to the point. Specify the direction of the positive Y axis.
     

    Normal to Curve at Point

    Select:

    		A nonlinear edge or sketch curve (arc, circle, ellipse, or spline) and a vertex, edge midpoint, sketch point, or work point on the curve.

    Result:

    The new work plane is normal to the curve and passes through the point.

     

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