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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How to Share a Sketch in Autodesk Inventor

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: HOW TO SHARE A SKETCH IN 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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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.

I hope this was helpful. Please drop comments and suggestions. They are highly welcome. Don’t forget to tell your friends about the site. Thanks.