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.
Work points can be placed or projected onto part faces, linear edges, or onto an arc or circle. Work points can be constrained to the center points of arcs, circles, and ellipses.
When creating 3D sweeps, you can place a work point at the intersection of work axes and work planes. You click work points and vertices of existing parts to define the path of the sweep.
Grounded work points have all degrees of freedom removed and are therefore fixed in space. An ungrounded work point can be repositioned by dimensions or constraints.
In a part file, use the Grounded Point command. When you create a grounded work point in a part file, the 3D Move/Rotate command is available so that you can specify certain operations relative to the grounded work point. Or, use the 3D Move/Rotate option on the context menu later to reposition the work point.
In an assembly, you first create a work point, right-click, and then select Grounded from the context menu. The 3D Move/Rotate command is not available in an assembly file.
To ground a work point in a part file, select it in the browser, right-click, and then select Ground.
If you clear the check mark on the Ground menu option, the associative relationship is restored. Changes to the selection geometry reposition the work point.
When you use Grounded Work Point on the Model tab, the created work point has no association to other geometry. It is fixed on the X, Y, and Z coordinates used to create it.
In a part file, right-click the grounded work point in the browser, and then choose one of the following options:
If geometry was used to position the work point, it is no longer associated to the work point. The work point remains grounded.
The work point becomes associative to new geometry that you select. Changes to the geometry reposition the work point.
On the Model tab, Work Features panel, use Point or Grounded Point in a part file to select model vertices, edge and axis intersections, intersections of three nonparallel faces or planes, and other work features as work points. You can also create work points as input to other work feature commands that require you to select a point.
In an assembly file, use the Point commands on the Model tab. Work points can be created at the intersection of part faces, edges, vertices, and work geometry that span hierarchical levels in the assembly.
Work points can be placed on holes and cuts in part faces, model surfaces, construction surfaces, and base surfaces. When Loop Select Mode is active, you can place a work point on one or more closed loops.
Prior to the introduction of Direct Manipulation modeling techniques in Inventor R2011, the Point command was the only method available to create work points. This legacy method was, and still can be, used with one of the methods described below:
Select two or more geometric elements to create a work point at the intersection of planes or the projection of two edges.
Assembly work points are placed at the bottom of the assembly hierarchy in the browser.
Specify X, Y, and Z coordinates to ground a work point. The work point remains fixed in space regardless of changes to model geometry. When creating a, in-line work features are not available.
You can fix a work point in 3D space in an assembly file. Changes to model geometry do not affect its position. All degrees of freedom are removed from the.
The 3D Move/Rotate command is not available in an assembly.
Although still valid, the Point 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 point creation.
Each of these new options is described on the Quick Reference tab of this Help topic.
A work point is a parametric construction point that can be placed on part geometry, construction geometry, or in 3D space. In an assembly, a work point cannot be created on the midpoint of a line.
Work points can be placed on holes and cuts in part faces, model surfaces, construction surfaces, and base surfaces. When Loop Select Mode is active, you can place a work point on any closed loop.
In a part, an ungrounded work point can be createdwhile using another work feature command. The Point command terminates as soon as the work point is created.
The Point drop-down menu offers the following work point creation options:
Point (legacy method)Select the appropriate model vertices, edge and axis intersections, or intersections of three nonparallel faces or planes to create a work point.
Grounded PointClick a work point, midpoint, or vertex. A pushpin cursor symbol indicates the selection is grounded.
On Vertex, Sketch point, or Midpoint
Select a 2D or 3D sketch point, vertex, or the endpoint or midpoint of a line or linear edge.
Intersection of Three Planes
Select three work planes or planar faces.
Intersection of Two Lines
Select any combination of two lines including linear edges, 2D or 3D sketch lines, and work axes.
Intersection of Plane/Surface and Line
Select a planar face or work plane and a work axis or line. Alternatively, select a surface and a sketch line, straight edge, or work axis.
Center Point of Loop of Edges
First, right-click and select Loop Select from the pop-up context menu. Then select one edge of a closed loop of edges.
Center Point of Torus
Select a torus.