Using the Sweep Tool (Swept Feature)

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

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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Using the Revolve Tool (Revolution Feature)

 

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

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 REVOLVE TOOL (REVOLUTION 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 using any unzipping utility.
3. Save the files 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: Understand and Using Sketch Linetypes and Geometry in Autodesk Inventor. It will help you understand terms like normal geometry, centerline geometry and construction geometry.

INTRODUCTION

Revolution is the process of sweeping a profile around a center axis. Revolution is used for creating parts that will be machined out through turning on a lathe machine. Such parts usually consists of circular features arranged around a common axis.
In Autodesk Inventor, a revolution feature is created using the Revolve tool. Table 1 shows examples of 2D sketches and the resulting models after a revolution operation. When creating a sketch that would be used for revolution, some facts have to be put into consideration. These include:

1. Imagine that the part to be created is sectioned longitudinally (that is, along its axis).
2. Sketch out the quarter-section of the part.
3. Draw a center line that represents the longitudinal axis of the part.
4. The center line should be drawn with the Centerline geometry settings toggled on.
5. When creating dimensions, dimension between the centerline and any other sketch geometry. This will create a diameter dimension that shows you the actual diametric dimension of the part.

It is also important to know when to use Revolve tool for creating circular features and when to use the Extrude tool for creating cylindrical features.

1. If you are creating a step shaft (that is, a shaft with varying cross-sectional areas along its longitudinal axis), then you should use the Revolve tool. This way, you will have an overview of the contour of the shaft from the beginning. You could easy make changes to the shaft profile just in one sketch.
2. If you are creating a simple shaft with a constant cross-sectional area, then it is very efficient to use the Extrude tool to create a cylinder feature that represents the shaft.
3. If you are creating a delicate circular model like a table-water bottle, then the Revolve tool will be the best tool to use. But your sketch must reflect all the delicate curves and grooves commonly found on such consumer products.

Table 1: A table Showing Different Sketches and Resulting Revolution Features

#	Sketch Geometry	Sketch and Resulting Model
1.	Triangular Sketch
2.	Rectangular sketch
3.	Rectangular sketch (with a gap between the profile and the axis)
4.	Any other profile.

OBJECTIVES

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

1. Explain the principle behind the creation of revolved features using the Revolution.
2. Use the Revolve tool for creating an Revolution Features.
3. Use the centerline geometry for defining the axis of revolution.

LOCATING THE REVOLVE TOOL

The Revolve tool could be found on:

1. RIBBON: Model tab > Create panel > Revolve
   
   
   
   
2. SHORTCUT: When you are in the Sketch environment and are through with the necessary sketches, simply press "R" on your keyboard to launch the Revolve tool.

With no further ado, let's get started. We are going to create a lot of revolved models, in order to enhance the understanding of the tool.
The dataset files contain base sketches for the models we are about to create. You could quickly use them for the exercises or create your own sketches from the scratch.

creating a centerline geometry

When you are creating a sketch that is meant to be revolved, it is advisable to uniquely define a line that will be used as the axis of revolution. This is often done by creating a line with a centerline geometry property. However, Inventor will works perfectly well with a line created with the normal geometry property. The difference is that when you explicitly define a single centerline in your sketch, Inventor will automatically recognise and select that centerline when you launch the Revolve tool. This way, your design intent is established right from the sketch and you will not pass through the hassle of selecting the axis of revolution when the Revolve dialog box comes on!

In case you are not familiar with the types of geometry in Autodesk Inventor, read this lesson: Understand and Using Sketch Linetypes and Geometry in Autodesk Inventor.

You can create a centerline geometry in two ways:

1. FROM AN EXISTING NORMAL GEOMETRY. In this method, you create the centerline as a normal geometry in the sketch environment. (Normal geometry are continuous, and are color-coded green when not fully constrained and navy blue when fully constrained.) After creating the normal geometry, click to select it. Go to the Format panel and click Centerline. This will toggle on Centerline for that particular geometry and effectively converts it to Centerline geometry.
2. DURING SKETCH GEOMETRY CREATION. In this method, you, first of all, go to the Format panel and toggle on the Centerline tool. Then go on and create the geometry as required. Inventor will create a centerline geometry. When you are through with creating the centerline, go back to the Format panel and toggle off the Centerline tool. I do not have to tell what will happen if the Centerline tool is not toggled off!

MODELLING A wheel CAP

In this exercise, we are going model a wheel cap for an infant scooter.

1. Open the dataset file using_revolve_tool-CAP.ipt. If you want to create the sketch yourself, refer to Figure 2 for the sketch.
   
   
2. Take some time to study the sketch. Take note of the normal geometry used for the profile that is to be revolved. Also take note of the centerline geometry, which will be used as the axis of revolution.
3. With the file opened, press "R" on your keyboard, or click Revolve on the Model tab > Create panel.
4. Inventor immediately selected the closed profile and the centerline, and displays a preview. Click OK to finish the revolution.
5. Orbit or change the view using the viewcube to see the other side of the model.

MODELLING AN INFANT-SCOOTER WHEEL

Let us create another revolved model. In this exercise, we are going model a wheel for an infant scooter.

1. Open the dataset file using_revolve_tool-WHEEL.ipt. If you want to create the sketch yourself, refer to Figure 3 for the sketch.
   
   
2. Take note of normal geometry, construction geometry, and centerline geometry used in the sketch. Also take note of the diametric dimension created between the centerline geometry and two of the normal linetype entities.
3. With the file opened, press "R" on your keyboard, or click Revolve on the Model tab > Create panel.
4. Inventor immediately selected the closed profile and the centerline, and displays a preview. Click OK to finish the revolution.
5. Orbit or change the view using the viewcube to see the other side of the model.

USING THE REVOLVE TOOL TO REMOVE A PORTION OF A MODEL

Just like the Extrude tool, we can use boolean operations (Join, Cut, Intersect) with the Revolve tool.

APPLICATION & DOCUMENT OPTIONS

Before we begin, let's customise our application and document:

1. Go to Tools tab > Options panel > click Application Options.
2. On the Application Options dialog box, click on the Sketch tab.
3. Ensure that the lower section of sketch settings are as shown in the image below. Click Ok to exit.
   
   
4. Go to Tools tab > Options panel > click Document Options.
5. On the Documents Options dialog box, click on the Sketch tab.
6. Set the X & Y Snap Spacing to 10mm. Click Ok to exit.
   
   
   

BASE SKETCH & BASE FEATURE

You could jump-start by opening using_revolve_tool-GROOVE-sketch1.ipt. Or you could follow the steps below:

1. Create a new part file using the template Standard (mm).ipt.
2. Create the sketch shown in Figure 4.
3. Make sure that the rectangle is centered around the Origin of the Sketch. Do the following:
   1. Ensure that you are looking at the sketch. Press "Page Up" on your keyboard and click Sketch1 on the Browser to Look At your sketch.
   2. On the sketch environment, go the Constraint panel > Horizontal constraint.
   3. Click the midpoint of the left vertical line and then click the sketch origin.
   4. On the Constraint panel, launch the Vertical constraint tool.
   5. Click the midpoint of the bottom horizontal line and then click the sketch origin.



4. Press "S" on your keyboard, or click Finish Sketch to exit the Sketch environment.
5. Press "E" on your keyboard to launch the Extrude tool. Set the distance to 200mm. Click OK to create the extrusion. Double click the mouse wheel to Zoom Extents. See Figure 5 for the base feature.
   

SECOND SKETCH & GROOVE

You could jump-start by opening using_revolve_tool-GROOVE-sketch2.ipt. Or you could continue with the steps below:

1. Right click on the top face of the base feature. Click New Sketch on the shortcut menu. Press "Page Up" on your keyboard and click Sketch2 on your Browser.
2. Create the sketch shown in Figure 6. Apply geometric constraints like symmetric and collinear to reduce the number of dimensions required to stabilise the sketch. Make sure the bottom line of the sketch passes through the sketch origin (as highlighted in Figure 6).
   
   
3. Select the four reference geometry that were auto-projected on sketch creation. Click Construction on the Format panel. This converts the reference geometry to reference construction geometry.
4. Select the vertical line passing through the center of the sketch. Convert it to a construction geometry.
5. Press "S" on your keyboard to exit the sketch environment. Your sketch is ready.
6. Press "E" to launch the Extrude tool. Set the Boolean operation to Cut and Extents Distance to 150mm. Click Ok to create the extrusion.
7. Orient the model using the viewcube the orientation shown in Figure 7.
   
   

THIRD SKETCH AND REVOLVED GROOVE

You could jump-start by opening using_revolve_tool-GROOVE-sketch3.ipt. Or you could continue with the steps below:

1. Click on the inner face of the groove (highlighted in Figure 7). Right click and select New Sketch on the shortcut menu.
2. Press "Page Up" on your keyboard and click on Sketch3 on your Browser. Press "F7" on your keyboard to slice the sketch.
3. Refer to Figure 8 and select the 7 reference geometry shown in light blue. Convert them to construction geometry.
4. Draw a vertical line passing through the center of the sketch. Use the midpoint of the bottom horizontal line as the start point. Convert it to a centerline geometry (See Figure 8).
   
   
5. Now draw two normal lines from point A to B and from point C to D as shown in Figure 9. These two lines will help in closing the sketch, else we won't be able to create a solid revolution.
   
   
6. Press "F6" to view the sketch in the Home View.
7. Press "R" to launch Revolve tool. Set the Boolean options to Cut and leave the Extents at Full. See Figure 9.
   
   
8. Click Ok to create the revolution. See Figure 10.
   
   
9. Compare your result with using_revolve_tool-GROOVE-completed.ipt.

This is the end of a long tutorial. I took tremendous time to develop the tutorial so that new users could follow up. If you did not understand some concepts, please refer to the Table of Contents page for other introductory lessons. Cheers!

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 the Extrude Tool (Extrusion Feature) - Part II

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PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

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 EXTRUDE TOOL (EXTRUSION FEATURE) - PART II

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 using any unzipping utility.
3. Save the files to a project folder of an existing Inventor project. Set the project active. Learn more about Inventor Projects and Project Files.

INTRODUCTION

This is the continuation of the lesson "Using th Extrude Tool (Extrusion Feature)." In this lesson, we are going to explore other Extents options found in Extrude dialog box in Autodesk Inventor. An understanding of the uses of each of the Extents options is important especially when complex designs are being created.

EXTENTS OPTIONS

The Extents options determine the methods for ending an extrusion and set its depth. Extrusions can be a specific depth or can terminate on a work plane, construction surface, or part face (including planar, cylindrical, spherical or toroidal face). The Extents options include:

1. Distance,
2. To next face/body,
3. To selected face/point,
4. Between two faces/planes,
5. Through All.

DISTANCE
The distance option extrudes in one direction only. It is the default option for creating extrusions in Inventor. With this option, the extrusion distance is simply typed into the value input box. One can combine the distance option with the direction controls (Direction 1, Direction 2, Symmetric, and Asymmetric) to achieve the desire extrusion. Most of the extrusion done in the first part of this lesson were carried out using the Distance option.
TO NEXT BODY/FACE
This option is used when the extrusion is desired to terminate at the next possible face or plane in the specified direction. This option is not available for base features or assembly extrusions.

1. Open the file Front_Frame_Extrusion_Lesson 2.ipt. The model contains an unconsummed sketch.
2. Re-orient the view as shown in Figure 2.
3. Launch the Extrude tool and set the Extents to To Next Body/Face. Click OK.
4. The Resulting solid is shown in Figure 3.

TO SELECTED FACE/POINT
Part Environment: When you choose To Selected Face/Point, next, select an ending point, vertex, face, or plane on which to terminate the extrusion. For points and vertices, the extrusion will be terminated on a plane parallel to the sketch plane which passes through the selected point or vertex. For faces or planes, the extrusion will be terminated on the selected face, or on a face that extends beyond the termination plane.
Assembly Environment: For assembly extrusions, sketch points, vertices, faces, and planes that reside on other components can be selected. Work planes and work points must reside on the same assembly level as the assembly extrusion being created to be selected.
If you terminate the extrusion on a face or plane, use options on the More tab to indicate a more specific solution when termination options are ambiguous, such as on a cylinder or irregular surface. On the More tab, Alternate Solution flips direction, selecting the termination face at the maximum distance. Select Minimum Solution to terminate on the first encountered face.
BETWEEN TWO FACES/PLANES
Part Environment: For part extrusions, selects beginning and ending faces or planes on which to terminate the extrusion.
Assembly Environment: For assembly extrusions, selects a face or plane on which to terminate the extrusion. Faces and planes that reside on other components can be selected. The selected faces or planes must reside on the same assembly level as the assembly extrusion being created. Not available for base features.
After you select the start and termination planes, use options on the More tab to indicate a more specific solution when termination options are ambiguous, such as on a cylinder or irregular surface. On the More tab, Alternate Solution flips direction, selecting the termination face at the maximum distance. Select Minimum Solution to terminate on the first encountered face.

1. Open the file Front_Frame_Extrusion_Lesson 3.ipt. The model contains an unconsummed sketch and two work planes.
2. Launch the Extrude tool. Click inside the smaller chord as the extrusion profile. See Figure 4.
3. For Extents, choose Between Two Faces/Planes.
4. For Starting plane/face, select the inner work plane (shown in green in Figure 4).
5. For Ending plane/face, select the outer work plane (shown in blue in Figure 4).
6. Clik OK to finish. The completed feature is shown in Figure 5.

THROUGH ALL
The Through All option is used to extrude the profile through all features and sketches in the specified direction. We have demonstrated this option in previous lessons.
REFERENCES

1. Autodesk Inventor 2011 Help System.

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 the Extrude Tool (Extrusion Feature)

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PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

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 EXTRUDE TOOL (EXTRUSION 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 using any unzipping utility.
3. Save the files to a project folder of an existing Inventor project. Set the project active. Learn more about Inventor Projects and Project Files.

INTRODUCTION

Extrusion is simply defined as the process of giving a 2D sketch a perpendicular height. That means converting the 2D sketch to a 3D entity; if your sketch was drawn on the X-Y plane, then your extrusion will proceed in the Z direction (which is perpendicular to the X-Y plane). You could also say that: extrusion is the process or technique of adding a height to a 2D sketch, thereby, effectively creating a 3D model.

In Autodesk Inventor, the extrusion process creates extruded features, and is carried out through the Extrude tool. The table below shows examples of 2D sketches and the resulting models after an extrusion operation.

Table 1: A table Showing Different Sketches and Resulting Extrusion Features

#	Sketch Geometry	Sketch Image	Resulting Extrusion Feature
1.	Circle		Cylinder
2.	Rectangle
3.	Other Geometry
4.	Any open sketch		Note: When an open profile is extruded, the result is always a surface.

You might need to make references to the following lessons in order to understand this lesson:

Understanding Constraints in Autodesk Inventor - Part 1

Understanding Constraints in Autodesk Inventor - Part 2

Understand and Using Sketch Linetypes and Geometry in Autodesk Inventor

Types of Features in Autodesk Inventor

OBJECTIVES

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

1. Explain the process of extrusion.
2. Understand the principle of the Extrusion Feature in Autodesk Inventor.
3. Use the Extrude tool for creating an Extrusion Feature.
4. Understand the uses of the Join, Cut, and Intersect options of the Extrude dialog box.

LOCATING THE EXTRUDE TOOL

The Extrude tool could be found on:

1. RIBBON: Model tab > Create panel > Extrude
   
   
   
   
2. SHORTCUT: When you are in the Sketch environment and are through with the necessary sketches, simply press "E" on your keyboard to launch the Extrude tool.

BASE SKETCHES & FEATURES

A Base Sketch is the first sketch found on your Model Browser, irrespective of its name. It is the first sketch that was created in the model.

A Base Feature is the first feature created from the base sketch. The base feature is usually a sketched feature (i.e. Extruded, Revolved, Swept, or Lofted features).

CREATING EXTRUDED FEATURES

In this lesson, it is assumed that you are familiar with Inventor's Sketch environment. If you are new to Inventor's Sketch environment, you might have to read previous lessons in this blog. Check out the Table of Contents. The tutorial was created with Inventor 2011.

You might want to read the tutorial on "Boolean Operations in Autodesk Inventor."

In this section, we are going to create a Front Frame part for an infant scooter.

BASE FEATURE

1. Open the dataset file Front_Frame_Extrusion_Lesson.ipt. The file was created with Inventor 2011 to ensure compatilibility with newer versions of Inventor.
2. Press E to launch the Extrude tool. Alternatively, go to Model tab > Create panel > Extrude tool.
3. Click on the Left and Right profiles. Set the extrusion distance to 60mm, and click OK to finish.

This is the base feature.

SECOND SKETCH AND FEATURE

Now, we are going to create a second sketch and second feature.

1. Click on the right-hand side of the base feature as shown in Figure 3. Click Create Sketch on the mini-toolbar to create a new sketch using the selected planar face.
2. Press Page Up and click on the planar face shown in Figure 3 to Look At the face.
3. Create the geometry as shown in Figure 4.
4. Launch Project Geometry: Sketch tab > Draw panel > Project Geometry.
5. Project the edges of the face next the face on which the current sketch is based. Refer to Figures 5 and 6 for guidance.
6. Next we convert all the projected (or reference geometry) to construction geometry. Select all the projected geometry.
7. Go to Sketch tab > Format panel and click Construction. See Figure 7.
8. Apply geometric constraints as shown in Figure 8. The completed sketch should be as shown in Figure 9.







9. Now, we are through with our sketch. Let's create the extrusion. Press E to launch the Extrude tool.
10. On the Extrude dialog, set Extents to All. Also set the Boolean operation to Intersect.
11. Click OK to finish the extrusion. The resulting solid is shown in Figure 10.

In the next lesson, we are going to explore the Extents options found on the Extrude dialog box.

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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Boolean Operations in Autodesk Inventor

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2011/2012/2013

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook | LinkedIn

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: BOOLEAN OPERATIONS IN AUTODESK INVENTOR

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 zipped file, and save the contents to a project folder of an existing Inventor project. Set the project active. Learn more about Inventor Projects and Project Files.
3. Take some time and familiarise yourself with Direct Manipulation in Autodesk Inventor. Check out this lesson: Direct Manipulation in Autodesk Inventor.

INTRODUCTION

A typical solid part is often made up of numerous features that are craftily combined to form the model. When, you are creating such a model in a CAD application like Inventor or AutoCAD, you have to split the modelling operation into various stages. A good designer should be able to quickly determine the feature that should be created first, and those that should be created subsequently. The subsequent features would be combined with the first feature (usually called the base feature) with the help of join, cut, or intersect operations. These are the Boolean Operations in Autodesk Inventor: JOIN, CUT, and INTERSECT. The Boolean Operations are found in the Extrude, Revolve, Loft, and Sweep tools.

OBJECTIVES

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

1. Describe the reason for the using boolean operations in your design workflow,
2. Describe the three basic boolean operations used in Autodesk Inventor,
3. Create simple models using these boolean operations.

JOIN OPERATION

The JOIN operation is used for joining a sketched solid feature to an existing solid feature. The result is a bigger solid that consists of all the volume enclosed by the newly formed sketched feature and the existing solid. In simpler terms, use the JOIN operation to add more features to your base feature.

Let's have some fun, by creating the Gland part shown above.

BASE FEATURE

We are going to start by creating the base of the Gland part. The dataset file already contains the base sketch for the Gland.

1. Open the file Gland.ipt from the extracted zipped file.
2. Press F6 to set the view to the Home view.
3. Press "E" on your keyboard to launch the Extrude tool (or go to Model tab > Create panel > Extrude tool on your Ribbon).
4. Set the Extrusion distance to 14mm and click OK or the green tick mark.

CREATING A NEW SKETCH USING A PLANAR FACE

Now, we are going to create a new sketch on the top face of our base feature.

1. Click the top of the base feature. The Direct-Manipulation mini-toolbar is display. Click Create Sketch.
2. Press Page Up and click the top of the base feature to Look At the new sketch.
3. In the Sketch environment, press C to launch the Circle tool. Click the centerpoint of the sketch as the center of the circle.
4. Type 55 as the diameter of the circle, and press the Enter key.
5. Press F6 to view the sketch in the Home view. Press E to launch the Extrude tool.
6. To select your extrusion profile, click inside the 55-mm diameter circle. Use 14mm as the extrusion distance. Leave other settings as they are. Use Figure 4 as your reference.
7. Click OK to finish the feature.

CUT OPERATION

The CUT operation is used for cutting a sketched feature from an existing solid feature. The result is a new solid that encloses the volume enclosed by the original solid but not by the newly formed sketched feature. In other words, the CUT operation subtracts the volume defined by the new sketched feature from that of the original sketched feature.

Let's demonstrate this by creating a hole from the center of our Gland part.

1. Click on the top face of the newly-created cylindrical feature. Click Create Sketch.
2. Press Page Up and select the top face of the cylinder to Look At the Sketch. Press C to launch the Circle tool.
3. Click the center of the sketch as the center of the circle, and type 36 as the diameter of the new circle.
4. Press F6 to return to the Home view. Press E to launch the Extrude tool.
5. Click within the 36-mm circle as the profile.
6. Click the Distance Arrow manipulator and drag it downwards, making it cut through the solid model (See Figure 6).
7. Go to the In-Canvas Display > Extents control > Select Through All.
8. Click OK.
9. Go on and add other features. Have fun.

Points to Note:

1. By clicking and dragging the manipulator through the existing solid, the system changes the boolean mode from Join to Cut. Drag the manipulator above and through the model and observe the subtle changes in the Extrude dialog box.
2. You could explicitly specify the Cut operation by clicking Cut on the Extrude dialog or via the In-Canvas display.

INTERSECT OPERATION

The INTERSECT operation creates a new feature or solid by retaining the volume common to the existing sketched feature and the newly formed sketched feature.

Let us create an interesting design using the INTERSECT operation.

1. Open the file DataSet_Intersection.ipt. The file contains an extruded feature and an unconsumed sketch.
2. Reorient the view to appear as shown in Figure 8. Use the ViewCube.
3. Press E to launch the Extrude tool.
4. On the Extrude dialog box, click on Intersect. Also select All on the Extents group. Refer to Figure 9.
5. Click OK to finish the extrusion.
6. Click the visible work plane. Right click and click Visibility to make it invisible.

Now, you can appreciate the power of INTERSECTION. Go on and have fun. Think about any other crafty feature you could create with the INTERSECTION operation.

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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