Boolean Operations in Autodesk Inventor

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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Using the Extrude Tool (Extrusion Feature)

Using the Extrude Tool (Extrusion 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 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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Using the Extrude Tool (Extrusion Feature) - Part II

Using the Extrude Tool (Extrusion Feature) - Part II-->

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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How to Share a Sketch in Autodesk Inventor

How to Share a Sketch in Autodesk Inventor

INTRODUCTION

For sketched features to be created, Autodesk Inventor require visible sketches. And more often, a sketch could contain geometry and loops that can be reused across many features. After the first sketch feature is created, the sketch is consumed by that feature and must be shared if other features must have access to the sketch. Sharing of sketches in the simplest way of reusing sketches and saving lots of time.

OBJECTIVES

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

1. Create a simple sketch in Autodesk Inventor,
2. Constrain the sketch with dimensional and geometric constraints,
3. Create an Extrusion feature, and
4. Share an existing sketch.

SHARING A SKETCH IN AUTODESK INVENTOR

CREATING THE SKETCH GEOMETRY

Let's begin this section by drawing a simple sketch with Inventor. Do the following (refer to Figure 1 for the completed sketch):

1. Launch Inventor. When Inventor is open, click CTRL + N, to launch the New File dialog box.
2. Go to the Metric tab of the New File dialog box, and select Standard (mm).ipt template. Click OK to create a new part file.
3. Press C to start the Circle tool. Create a circle of diameter 20mm that is centered on the sketch.
4. Start another circle that is centered on the upper-left side of the first circle (Refer to Figure 2). Draw the circle towards the circumference of the first circle. A tangent constraint is inferred. Click the circumference of the first circle while the glyph is still showing.
5. Repeat step 4 and draw another circle centered at the upper-right side of the first circle. (Refer to Figure 3 for guidance.)
6. Press L to launch the Line tool. Create a horizontal line above the two top circles.
   
   
   
   

CONSTRAINING THE SKETCH

1. Now, on the Sketch tab > Constrain panel, launch the Coincident Constraint tool.
2. Click the left endpoint of the line and click the left circle.
3. Repeat step 8 for the right circle.
4. On the Sketch tab > Constrain panel, launch the Tangent Constraint tool.
5. Click the line and the left circle.
6. Repeat step 11 for the right circle.
7. On the Sketch tab > Constrain panel, launch the Equal Constraint tool.
8. Click the left and right circles.
9. Press D to launch the Dimension tool. Click the left circle. Apply a dimension of 25 mm.
10. Click the line and the centerpoint of the center circle. Click the 25-mm dimension that was applied to the left circle. Press Enter. A reference dimension is created.
11. The status bar should be displaying "fully constrained."
12. On the Sketch tab > Modify panel, launch the Trim tool. Click the inner segment of the center circle to trim it off. (Refer to Figure 1 for guidance).
13. Press S to exit the sketch environment. Save the file.

CREATING THE EXTRUSION FEATURE

1. At the upper-right corner of the Graphics Area, click the Home icon on the Viewcube.
   
   
2. Press E to launch the Extrude tool. The Extrude dialog box is displayed. The sketch has three closed profiles (or loops). So Inventor can not automatically select anyone for you. Select all the three profiles. Note that you can remove a profile by holding down CTRL and reselecting the profile.
3. On the Shape tab > Extents area, type 10mm as the height of extrusion.
4. Click OK to create the Extrusion1 feature (confirm the name from your Model Browser). Sketch1 is now consumed by Extrusion1.

SHARING SKETCH1

1. On the Model Browser, expand the Extrusion1 feature. Sketch1 is seen to be located under Extrusion1.
2. Right click Sketch1. On the shortcut menu, click Share Sketch. (See Figure 5)
3. Sketch1 is shared and is now added as a first-level object on the Model Browser. (See Figure 6).






4. Click the Home icon on the Viewcube. (See Figure 4).
5. On the Navigation bar, launch the Orbit tool. (See Figure 7)
   
   
   
   HOT TIP: You can also execute the Orbit tool by Holding down the Shift key and Press and drag the mouse wheel on a 3-button mouse.
   
6. Click and drag the center of the reticle ( See Figure 8) and reorient the model to appear as shown in Figure 9
   
   
   
   
   

CREATING ANOTHER EXTRUSION FEATURE

1. Press E to launch the Extrude tool. Sketch1 has been shared, so we reuse it for creating another sketched feature.
2. Click the central profile, and use 20 mm as the height of extrusion. Click the direction 2 button to flip the direction upwards if it's directed downwards.
   
   
3. Click OK to finish the Extrusion2 feature.
4. Right click Sketch1 on the Model Browser, and click Visibility to turn off the visibility of the sketch. Save the file.
5. The model is completed.
   
   

This method can be used for creating very complex parts from one sketch. But it's also a good workflow to create the sketches when needed.
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

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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