Using and Understanding Work Planes in Autodesk Inventor Professional

Platform: Autodesk Inventor Professional

Level of Difficulty: Beginners

Author: Ndianabasi Udonkang

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Overview

Work features are modeling aids. From the first sketch to the last feature of your model, work features are used to aid the modeling process. And as the design becomes more complex, you will need the help of work features to find your way out! These work features can be used for creating sketches, for constraining of components in the assembly environment, for feature termination (in both part and assembly designs), and for creating other work features.

There are three types of work features in Autodesk Inventor, namely:

1. Work planes;
2. Work axes; and
3. Work points.

Every part or component in Autodesk Inventor has a default set of work planes, work axes, and work point. These default work features are located in the Origin folder of the Model browser. The default work planes correspond to the XY, XZ, and the YZ planes. The default work axes correspond to the X, Y, and Z axes, while the default work point correspond to the Center Point as seen in the origin folder of any part or assembly file. The Center Point is the origin of the part, i.e., it is the "owner" of 0,0,0 coordinate. It is located at the intersection of the X, Y and Z axes.

 

Visibility of Work Features

The visibility of work features can be controlled individually or globally. When controlled individually, only the selected work feature is affected but when controlled globally, the visibility of all features are affected simultaneously. For instance, if you wish not to see any work axis in your sketch or model environment, simply turn off the global visibility for work axis. And if you simply do not want to see a particular work plane, just turn off the visibility for that work plane.

Controlling work-feature visibility individually

When a work feature has been used to achieve its purpose, it is a good housekeeping practice that such a feature is turned off. These are the steps:

1. Select the affected work feature(s).
2. While the feature(s) are still selected, right-click on the browser or graphics window.
3. On the context menu, click on Visibility, to uncheck it.
4. These steps could be followed when you want to turn on the visibility as well.

Controlling work-feature visibility globally

Now, they are times you are just fed up with seeing all the work features taking up valuable real estate on your graphics windows, and they are so many that you just cannot turn them off individually, then, at times like these, the globally control becomes indispensable. To turn off work features off globally, follow the following procedures:

1. On the Ribbon, go to the View tab, Visibility panel, Object Visibility flyout.
2. On the flyout, uncheck the checkbox (es) that correspond to the object whose visibility you wish to turn off globally.
3. Uncheck All Workfeatures, to turn off the visibility of all work planes, work axes, work point, and UCS triad.
4. Alternatively, you can use the following keyboard shortcuts to turn off the global visibility of work features:
1. Alt + ] (toggles the visibility of work planes)
2. Alt + / (toggles the visibility of work axes)
3. Alt + . (toggles the visibility of work points).

Working with Work planes

Work planes are primarily used to define a planar surface for creating new sketches for model, or components. When you create or define a work plane based on existing geometry of a model, it is parametrically linked to the model, ensuring that the plane updates if changes are made to the model.

Applications Of Work Planes In Modeling

1. Work planes are used for defining the orientation of new sketches.
2. Work planes are used for feature termination, that is, they could be used for defining where the termination plane for extrusion features.
3. Work planes are used as the basis for creating other work features ( work planes, axes, or points).
4. Work planes are also used for constraining components to components in the assembly environment.

Techniques for Creating Work Planes

There are many techniques for creating work planes and their usage depends on the shape of the model, the orientation of the model relative to the default work features, and the availability of custom work features. One important advice I would like to give is that, you should always try to center the base sketch of any component about the origin of the sketch. When this is done, default work features can be used if they satisfy your needs.

Method 1: Creating an Offset Work Plane from an Existing Plane

This method is used for creating a parallel work plane at a distance from an existing work plane (default or user) or a face.

Procedure:

1. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
2. On the graphics window, go to the face you wish to offset. Left click, hold and drag upwards or downwards. Release the mouse button and type in the precise value for the offset in the textbox shown on the screen. Click Enter to return the value. An offset plane will be created.

Method 2. Creating a Work Plane at the Midplane between two Parallel Planes

This method is used for creating a work plane at the midplane between two parallel work planes or faces.

Procedure:

1. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
2. Click on the two faces or planes you wish to use. A parallel plane will be created at the midplane between the two faces or planes.

Method 3. Creating a Work Plane at an Angle to a Face or Plane about an Edge

This technique is used for creating a work plane that will be inclined an a specified angle from face or plane about an edge or axis.

Procedure:

1. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
2. Click on the reference face or plane. Note that the angle will be calculated or counted from this face or plane.
3. Click on the axis or edge about which the new plane will be rotated or inclined.
4. Type the numerical value or expression for the angle in the input box shown. Note that negative values are also accepted and these will reverse the direction of rotation.
5. Click OK or Enter. The work plane will be created at the specified angle from the reference face or plane about the specified direction.

Method 4. Creating a Work Plane Tangent to a Surface and Parallel to a Plane

This method is used for creating a work plane that will tangent to a surface and parallel to a specified plane. This plane could be any of the default plane or a user-defined work plane.

Procedures:

1. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
2. On the Model Browser, expand the Origin folder to reveal the default work planes.
3. Select the default plane you want the new work plane to be parallel to. Note that you can also use user-defined work planes.
4. Click on the surface you want the new work plane to be tangent to.
5. The required work plane is created.

Method 5. Creating a Work Plane passing through Three Points or Vertices

This method is used for creating a work plane that will pass through three work points or vertices of a component.

Procedure:

1. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
2. Click on the three work points or vertices you want the work plane to pass through.
3. The required work plane is created.

Method 6: Creating a Work Plane passing through a Point and Tangent to a Surface

This method is used for creating a work plane that passes through a work point, endpoint¸ midpoint, or vertices and tangent to a surface.

Procedure:

1. On the Ribbon, go to the Launch panel and click on the New tool.
2. On the New File dialog box, go to the Default tab and double-click the template: Standard.ipt.
3. A new sketch is opened for the new part file.
4. Launch the Circle tool: Sketch tab > Draw panel > Circle.
5. Click on the sketch origin for the centre of the circle and draw a rough circle of any size.
6. Launch the Dimension tool: Sketch tab > Constrain panel > Dimension. Click on the circle; in the box type in 1 in (one inch).
7. Click Finish sketch on the Exit panel.
8. In the model environment, go to Create panel > Extrude. The single profile is automatically detected as the profile for the extrude operation. Match the parameters with the one shown in Figure 12. Click OK.

1. On the Model tab > Sketch panel, click on Create 2D Sketch tool. Select the top face of the cylinder as the sketch plane.
2. On the navigation bar at the right-hand side of the graphics window, click on the View Face tool. Click on the top face of the cylinder or click Sketch2 on the Model Browser.
3. On the Sketch tab > Draw panel, launch the Point tool. Click anywhere on the projected circular edge of the cylinder.
4. On the Constraint panel, launch the Vertical Constraint tool. Constraint the sketch origin vertically with the point that you created previously. On the Exit panel, click Finish Sketch.
5. On the model environment, with Sketch2 still visible, launch the Work Point tool on the Work Features panel. Click on the 2D point that was create on Sketch2. A work point is created on the circular edge of the cylinder. Press F5 to view the model in the home view. You may turn off the visibility of Sketch2.
6. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
7. Click on the cylindrical surface of the model and select Work Point1 on the graphics window or model browser. A tangential work plane is created passing through the work point.

Method 7. Creating a Work Plane Passing through Two Coplanar edges

This method is used for creating a work plane that passes through two coplanar edges, axes, or lines.

Procedures:

1. On the model environment, launch the Work Plane tool (Ribbon: Model tab > Work Features panel > Work Plane tool) or use the keyboard shortcut: ].
2. Click on the first and second edges you want the work plane to pass through.
3. A work plane passing through the selected coplanar edges will be created.

Conclusion:

There are other ways of creating work planes, however, those presented above will be enough for most real-world problems. I hope you found the topic useful. Please drop a comment; it will be appreciated. Good luck.

These are the other lessons about work features; check them out:

• Using and Understanding Work Points in Autodesk Inventor Professional
• Using and Understanding Work Axes in Autodesk Inventor Professional
• Using and Understanding Grounded Work Points in Autodesk Inventor Professional

Understanding and Using Sketch Linetypes and Geometry

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners.

Author: Ndianabasi Udonkang

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In Autodesk Inventor, sketch linetypes are used to further enhance the capturing of design intent in the 2D sketch environment. Sketch geometry such as lines, circles, arcs, ellipses, rectangles, polygons, and splines can be assigned different linetypes for different purposes. There are four types of linetypes in Autodesk Inventor, namely:

1. Normal linetype;
2. Construction linetype;
3. Reference linetype; and
4. Centerline linetype.

Each of these linetypes, when assigned to geometry in the sketch environment, gives rise to the four types of sketch geometry, namely:

1. Normal sketch geometry;
2. Construction geometry;
3. Reference geometry; and
4. Centerline geometry.

 

Normal Linetype and Geometry

When geometry is initially sketched, it appears with a continuous linetype. This is called normal sketch geometry. The normal linetype is the default linetype for sketch geometry unless the centerline or construction linetypes tools have been activated on the Format panel of the Sketch tab. Normal linetypes are primarily used for defining profiles, path, and guide rails for sketched features. [Note: Sketched features are those features that are derived or generated from sketches. They include extruded, revolved, lofted, and swept features.]

In Figure 2, a sketch, consisting mainly of normal linetype geometries, is shown.

Construction Linetype and Geometry

The construction linetype is used to represent geometry that would not directly participate as profile, path, or guide rails of sketched features. Construction geometry is used for as aid for constructing and constraining normal geometry. Construction geometry is vital in capturing design intent. For example in Figure 3, a construction line is used to define the size of the entry slot of a machine clip.

Creating Construction Geometry

Use the following steps to create construction geometry.

1. In the Sketch environment, go to Sketch tab > Format panel and click the Construction tool.
2. On the graphics windows, create any geometry your choice, the geometry will be displayed as a construction geometry.
3. Deactivate the construction geometry mode by clicking on the Construction tool on the Format panel and continue drawing normal geometries.

Converting Existing Geometry to Construction Geometry

If you’ve already drawn geometry and you wish to convert it to construction geometry, follow these steps.

1. On the graphics window, select the geometry you want to convert to construction geometry.
2. Go the Sketch tab > Format panel and click the Construction tool. The geometry is converted to construction geometry.

This method is the fastest and ensures that you do not forget to deactivate the construction mode when using the first method.

Centerline Linetype and Geometry

The centerline linetype is used for creating centerline geometry. When centerline geometry is placed in a sketch, it is automatically recognized by the Revolve tool as the “Axis of Revolution.” When a dimension is placed between a centerline geometry and other geometries, a diameter dimension is automatically created.

Creating Centerline Geometry

Use the following steps to create construction geometry.

1. In the Sketch environment, go to Sketch tab > Format panel and click the Centerline tool.
2. On the graphics windows, create any geometry your choice, the geometry will be displayed as a centerline geometry.
3. Deactivate the centerline geometry mode by clicking on the Centerline tool on the Format panel and continue drawing normal geometries.

Converting Existing Geometry to Centerline Geometry

If you’ve already drawn geometry and you wish to convert it to centerline geometry, follow these steps.

1. On the graphics window, select the geometry you want to convert to centerline geometry.
2. Go the Sketch tab > Format panel and click the Centerline tool. The geometry is converted to Centerline geometry.

Reference Geometry

Reference geometry is created by projecting part faces, edges, and vertices onto the current sketch plane. Sketch geometry belonging to another sketches and work features ( such as work point and work axis) can also be projected to the current sketch. Reference geometry is the best way to ensure that a sketch is linked parametrically to an already existing part or sketch. Reference geometry remains associative to the original part vertices, edges, faces, and work features. Reference geometry can be used to define the profile or path for a sketched feature.

Properties of Reference Geometry

1. Reference geometry cannot be dimensioned.
2. It cannot be trimmed
3. It can be mirrored
4. It cannot be drawn. However, it can be created by using the Project Geometry tool or activating the Autoproject Edges option on the Application Option dialog box.

Creating Reference Geometry

Autoproject Options

Reference geometry is created automatically when you use a planar face of an existing part as the sketch plane. The edges of the selected face are projected on to the new sketch, but this depends on the Autoproject Options on the Application Option dialog box. To activate the Autoproject Option, follow these steps.

1. On any environment, go to the Ribbon > Tools tab > Options tab > Application Options tool.
2. On the Application Options dialog box, click on the Sketch tab and go to the lower section. Check the checkboxes with the labels: “Autoproject edges for sketch creation and edit” and “Autoproject edges during curve creation.”
3. Click Apply and close.

 

Autoproject edges during curve creation

When this checkbox is activated on the Application Options dialog box, edges of existing parts can be projected on to sketch plane during sketching by hovering the cursor over them.

Autoproject edges for sketch creation and edit

When this checkbox is activated on the Application Options dialog box, the edges of planar faces are projected on to the current sketch plane.

Project Geometry Tool

The Project Geometry tool is used to project additional part faces, edges, vertices, and work features on to the sketch plane as reference geometry. When the Project Geometry tool is launched, you are asked to select the faces, edges, vertices, or work features that will be projected. One selected, the reference geometry is created on the current sketch plane which remain associative with the original faces, edges, vertices, or work features. By being associative, it means that the reference geometry depends on the original faces, edges, vertices, or work features and will update if they are changed.

To create reference geometry using the Project Geometry tool, follow these steps:

1. On the Sketch tab of the sketch environment, go to Draw panel > Project geometry tool.
2. Select the faces, edges, vertices, and/or work features of interest. Reference geometry is created on the current sketch plane.

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