Using the Sweep Tool (Swept Feature)

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

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This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series

TOPIC: USING THE SWEEP TOOL (SWEPT FEATURE)

BEFORE YOU BEGIN

1. Download the dataset. The dataset files were created with Inventor 2011 to ensure compatibility with newer versions of Inventor.
2. Extract the content of the zip file using any unzipping utility.
3. Save the extracted file to a project folder of an existing Inventor project. Set the project active. Learn more about Inventor Projects and Project Files.
4. Go through the tutorial: Using and Understanding Work Planes in Autodesk Inventor. It will help you understand how to create work plane, which is important for creating with swept features.

INTRODUCTION

Swept features are one of the sketched features found in Autodesk Inventor. Swept features are created with the Sweep Tool. The term "sweep" in the context of swept features means extruding a sketch along a path, or curve. While the "Extrude Tool" sweeps along a straight line, the "Sweep Tool" sweeps the profile along the specified curve. The curve could be a straight line or any other complex two-dimensional or three-dimensional path. The Sweep tool requires two unconsumed and visible sketches in order to create a swept feature. One of the sketches must contain the profile to be swept (profile sketch), while the other sketch must contain the curve along which the profile will be swept (path sketch). The path sketch could be a 2D sketch or 3D sketch.

OBJECTIVES

At the end of this lesson, the reader should be able to:

1. Explain the concept of sweeping and swept features.
2. Use the Sweep tool for creating a Swept Feature.
3. Create a work plane that is parallel to an existing plane but coincident with a point along a path.

LOCATING THE SWEEP TOOL

The Sweep tool can be found on:

1. RIBBON: Model tab > Create panel > Sweep
   
   

CREATING A WORK PLANE FOR SWEPT PROFILES

One of the important techniques to be mastered when one is considering creating a swept feature is that of creating of work planes. Work planes are the basis for creating the profile and path sketches. You could start by creating the profile sketch first and the path sketch later, or vice versa. The choice is yours.

In this section, we are going to create a work plane and then create a path sketch on that work plane. The dataset file, using_sweep_tool_handle_3D_sketch.ipt, contains two 2D sketches containing 2D points which are used for creating a 3D sketch. We are going to create a work plane which is concident with the right endpoint of the 3D curve and parallel with th XZ plane (See Figure 2).

Let us now create the work plane.

CREATING THE WORK PLANE

1. Open using_sweep_tool_handle_3D_sketch.ipt.
2. Go the Model tab > Work Features panel > Plane. Click the flyout below Plane and select Parallel to Plane through Point (See Figure 3).
   
   
3. Expand the Origin folder and click on the XZ plane (See Figure 4). Next click the right endpoint (highlighted in Figure 2).
   
   
4. A new work plane is created.

Next we create a profile sketch on the newly-created work plane.

CREATING THE PROFILE SKETCH & THE SWEPT FEATURE

1. Right click on the newly-created work plane on the graphics window. Click New Sketch on the shortcut menu. A new sketch is created.
2. Refer to Figure 5. Click View Face on the Navigation Bar and click the name of new sketch (Sketch3 or Sketch4, depending) on the Model Browser.
3. Create two concentric circles with diameters 30mm and 26mm (as shown in Figure 5).
4. Click Finish Sketch and press "F6" on your keyboard.
5. Click Sweep on the Create panel (See Figure 1).
6. See Figure 7. Click the region between the two concentric circles as your profile. Next click the 3D curve as your path. Click OK to create the swept feature.
7. Right click the work plane (still visible on the graphics window) and click Visibility on the shortcut menu to turn off its visibility.
8. The completed model is shown in Figure 8.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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Creating a Cylinder at an Angle to a Hemisphere

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2012

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series.

TOPIC: CREATING A CYLINDER AT AN ANGLE TO A HEMISPHERE

INTRODUCTION

This article was written as a reply to a question asked by one of my blog readers. He wanted to know how to draw a cylinder at an angle to a hemisphere as shown below.

So this was the reply:

CREATING THE CIRCULAR BASE

1. Create a new part file. A new sketch should open by default.
2. In the Sketch environment, sketch a circle (say diameter 100mm). Use the center of the sketch as the center of the circle.
3. Immediately press E to initiate the Extrude tool. Extrude to a height (say 5mm).

CREATING THE HEMISPHERE

1. Press S to launch the Sketch tool immediately. Click the top face of the circular base as the sketch plane. Sketch a semicircle (say of diameter 80mm). You can use the Arc tool(Center Point option).
2. Join the endpoints of the semicircle with a line. Constrain the line to pass horizontally through the center of the sketch. If necessary, use the Trim tool to clean up the sketch.
3. Make the line a centerline geometry. You can do this by selecting the line and clicking on the Centerline tool on the Sketch Tab> Format Panel.
4. Press R to launch the Revolve tool immediately. Set the angle of revolution to 180 degrees. Click Ok.

CREATING THE INCLINED CYLINDER

Now I'm assuming that you followed my procedure. By constraining the circle that was used to create the circular base to the center of Sketch1, I ensured that the feature is entered in the graphics area. So I can reuse some of my default work planes and work axes without creating unnecessary new ones.

1. On the Model Browser, expand the Origin folder. Right click the XZ Plane and click Visibility to make the XZ plane visible.
2. Repeat step 1 above to make the X Axis visible.
3. Press ] to launch the Work Plane tool. Click the XZ Plane and the X Axis (they should be visible on the graphics area). You can also select them through the Model Browser. This technique is used to create a work plane at an angle to a plane about an axis.
4. Now set the angle of rotation to say 125 degrees. Click OK. A work plane is created (let's call it Work Plane 1).
   
   Now we are going to create an offset work plane parallel to Work Plane 1.
   
   
5. Press ] to launch the Work Plane tool. Click and drag Work Plane 1 upwards above the hemisphere. Set the distance to say 50mm(Check if the distance is +ve or -ve. Also ensure that the new work plane is slightly above the hemisphere to your desired distance). Click OK. A new work plane is created. (Let's call it Work Plane 2.)
6. Now press S to launch the Sketch tool. Select Work Plane 2 as the sketch plane to use.
7. Create a circle of say diameter 25mm at the center of the new sketch.
8. Press E to launch the Extrude tool. On the Extrude dialog box > Shape tab > Extents Area, set the Extents to "To Next". Click Ok. A cylinder is created from the Work Plane 2 to the hemisphere.
9. Save file.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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Using and Understanding Grounded Work Points in Autodesk Inventor Professional

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners

Author: Ndianabasi Udonkang

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This is the last lesson in the series on using and understanding work features in Autodesk Inventor Professional. In this series we are going to learn how to use an important but often ignored tool called "grounded work point."

Overview

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 Work Planes in Autodesk Inventor Professional

Grounded work points are one of the work features available in Autodesk Inventor. Grounded work points are just work points that are not parametrically attached to any model or component in your design. Ordinary work points are created by constraining them to faces, edges, or points on our models so that if the model changes, the work point will also update. However, grounded points are created relative to the coordinate system of the assembly or part i.e. they are created by specifying their X, Y, and Z coordinates with respect to the origin of the part or assembly. Grounded work points can be created in both part and assembly environments.

In Model Browser, a pushpin is attached to a work point to indicate that it’s grounded.

Creating Grounded Work Points

Method 1 - Creating a Grounded Work Point directly from the Grounded Work Point tool

This method creates a grounded work point directly from the Grounded Work Point tool. Here you will be asked to first of all select the vertex you wish to initially place the grounded work point on. Later you may redefine it by entering precise coordinate inputs.

Procedure:

1. On the Model environment, go to the Work Features panel. Click the drop-down arrow beside the Work Point tool and select Ground Point on the drop-down menu. Alternatively, use the keyboard shortcut ";"
2. 
3. Select a work point or vertex to define the initial position of the grounded work point.
4. On the 3D Move / Rotate dialog box, click Apply to accept the initial position and orientation and create the grounded work point
5. 
6. Before clicking the Apply button, you may want to rotate the grounded work point about the X, Y, or Z axis. To do this, click any of the axes on the triad and rotate it to the desired angle. The magnitude of the angle will be shown dynamically on the 3D Move / Rotate dialog box
7. 
8. You may also like to enter precise coordinate values for the grounded work point. To do this, click on the Redefine alignment or position button on the 3D Move / Rotate dialog box and enter the precise X, Y, and Z coordinates.
9. 

Method 2 - Creating a Grounded Work Point from an existing Work Point

This method is used to convert a work point to a grounded work point.

Procedure:

1. Locate the existing work point on the Model Browser.
2. 
3. Right click on the work point and click Ground on the context menu. The work point is converted to a grounded work point and a pushpin is attached to it on the Model Browser.
4. 
   
   
5. 

Let me know your thoughts about the lesson. Why is useful? Are they area to improve on? Is there anything I failed to mention? What about my methodology? Just feel free to tell and I will appreciate it. Contact me via ndianabasi.udonkang@gmail.com. Thanks and God bless.

Using and Understanding Work Points in Autodesk Inventor Professional

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners

Author: Ndianabasi Udonkang

Follow me on Twitter | Facebook

 

This is the third lesson in our series about work features. In part 1, we learnt how to create work planes and in part 2, we learnt how to create work axes. In this lesson, we are going to learn how to create work points.

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

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

___________________________________________________________________________________

Overview

Work points are one of the work features in Autodesk Inventor. Work points are used extensively in part and assembly environments for defining centers of circular patterns, for assembly constraints, for 3D sweep, etc. These work points are parametrically attached to the models used for creating them so that if the model changes, the work points change too.

Applications of Work Points

1. Work points are used for defining the centers of circular patterns, and hole features.
2. Work points are used in the assembly environment for constraining one component to another.
3. Work points helps in the process of defining paths for 3D sweeps. Very important applications of this are found in the Cable &Harness and Piping & Tubing environments of Autodesk Inventor.
4. Work points can be projected onto a 2D sketch as a 2D point.
5. Work points are used for constructing other work features such as work axes and work planes.
6. Work points can be used for defining coordinate systems.

Techniques for Creating Work Points

Method 1 - Creating a Work Point on a 2D or 3D point, vertex, Endpoint or Midpoint of a Line or Linear Edge

This method is used for creating a work point on a 2D point of 2D sketch or 3D point of a 3D sketch. It is also used for creating a work point on a vertex of a component. A work point can be created on the endpoint or midpoint of a sketch or a linear edge of a component.

Procedure:

1. On the model environment, launch the Work Point tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: "."
2. On the graphics window, click the vertex you want to create the work point on. A work point is created on the vertex. OR

1. On the graphics window, click the midpoint of a linear edge. A work point is created on the specified location. Similarly,

1. On the graphics window, click a 2D or 3D sketch point. A work point will be created on the point. Note that the 2D sketch must be visible or unconsumed.

Method 2 - Creating a Work Point at the Intersection of Three Planes

This method is used for creating a work point at the intersection of three work planes or planar faces.

Procedure:

1. On the model environment, launch the Work Point tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: "."
2. On the graphics window, click on the three work planes (1,2 &3) or face to be used. A work point will be created at the intersection of the selected work planes.

Method 3 - Creating a Work Point at the Intersection of Two Lines

This method is used for creating a work point at the intersection of two lines or linear edges. For lines to used, a visible 2D or 3D sketch must be available.

Procedure:

1. On the model environment, launch the Work Point tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: "."
2. On the graphics window, click on the two lines or linear edges (1 &2) to used. A work point will be created at the intersection of these lines or linear edges.

Method 4 - Creating a Work Point at the Center of the Loop of Edges

This is a very smart method for creating work points. Many inventor users do not know that such a method exist. In this method you create a work point at the center point of a selected loop of edges.

Procedure:

1. On the model environment, launch the Work Point tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: "."
2. Right click on the graphics window and select "Loop Select" on the context menu.

1. On the graphics window point at any edge of the model, a loop will be pre-highlighted.
2. Select the desired loop and a work point will be created at the center of the loop.

Method 5 - Creating a Work Point at the Intersection of a Line with a Plane

This method is used for creating a work point at the intersection of a line or linear edge with a plane or face.

Procedure:

1. On the model environment, launch the Work Point tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: "."
2. On the graphics window, click on the plane (1) and the line or linear edge (2). A work point will be created at the intersection of the work plane and the edge.

Using and Understanding Work Axes in Autodesk Inventor Professional

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners



Author: Ndianabasi Udonkang

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This is the second lesson in the series. In the first part, we talk about using and understanding work planes. This lesson will focus on the use of work axes.

Overview

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

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

Work axes are construction tools used for marking the positions of centerlines, symmetry lines, or the center axes of revolved features. Work axes are also used for generating other work features – work planes or work points.

Application of Work Axes

1. For indicating centerlines on 2D and 3D sketches. Work axes can be projected on 2D sketches as centerlines for revolve features.
2. Work axes can be used for indicating the axis of revolution of circular patterns in both part and assembly modeling environment.
3. Work axes can be used for creating other work features.

Techniques for Creating Work Axes

Method 1. Creating a Work Axis Collinear with an Edge or Sketch Line

This method is used for creating a work axis that is collinear (or on the same line) with the edge of a model or a sketch line of an unconsumed sketch.

Procedure:

1. On the model environment, launch the Work Axis tool (Ribbon: Model tab > Work Features panel > Work Axis tool) or use the keyboard shortcut: “/”

1. On the graphics window, click on the edge of the model or sketch line you want the work axis to be collinear to. Note that to create a work axis that is collinear with a sketch line, there must be a visible sketch on the graphics window. To make use of a consumed sketch, go to the model browser, right-click on the name of the sketch and click “Share sketch” or turn on the visibility of the sketch. A work axis is created.

Method 2. Creating a Work Axis Parallel to a Line or Edge through a Point

This method is used for creating a work axis that is parallel to a Sketch Line or Edge and passing through a work point.

Procedure:

1. On the model environment, launch the Work Point tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: “.”
2. On the graphics window, click on a vertex to create a work point on the vertex. A work point is created.
3. 
4. On the model environment, launch the Work Axis tool (Ribbon: Model tab > Work Features panel > Work Axis tool) or use the keyboard shortcut: “/”
5. Click on the work point created in step 2 and then on an edge of the model. A work axis passing through the work point and parallel to the edge is created.
6. 

Method 3: Creating a Work Axis passing through Two Points

This method is used for creating a work axis that passes through two work points or vertices.

Procedure:

1. On the model environment, launch the Work Axis tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: “/”
2. On the graphics window, click on two work points or vertices you want the work axis to pass through. A work axis passing through the two specified points will be created.

Method 4. Creating a Work Axis at the Intersection of Two Planes

This method is used for creating a work axis that is coincident with the intersection of two faces or work planes.

Procedure:

1. On the model environment, launch the Work Axis tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: “/”
2. On the graphics window, click two “intersecting” faces or work planes. A work axis will be created at the intersection between them.

Method 5. Creating a Work Axis through a Revolved Face or Feature

This method is used for creating a work axis that passes through the longitudinal axis of a cylindrical face or feature.

Procedure:

1. On the model environment, launch the Work Axis tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: “/”
2. On the graphics window, point and click on a cylindrical face or feature. A work axis passing through the longitudinal axis of the face or feature will be created.

Method 6. Creating a Work Axis Normal to a Plane through a Point

This method is used for creating a work axis that is normal to a plane and passing through a point or vertex.

Procedure:

1. On the model environment, launch the Work Axis tool (Ribbon: Model tab > Work Features panel > Work Point tool) or use the keyboard shortcut: “/”
2. On the graphics window, click on the face or plane you want the work axis to be normal to.
3. Click on the point, work point or vertex you want the work axis to pass through. A work axis passing through the point and normal to the specified plane will be created.

Conclusion

I hope you found the tutorial useful. I will love to get comments about my writing style and content. You can email via ndianabasi.udonkang@gmail.com. Cheers.

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