Autodesk Inventor Hands-on Test Drive !$# Autodesk Part No.: 000000000000113652 Date: 10.02.03 Colors: 5-Color (CMYK+PMS 877) Description: Inventor 8 “Hands-on Test Drive” Manual Cover, Size: 6.312” (160.325 mm) wide x 9.062” (230.175 mm) high.
INV8_AddressPage2.fm Page 1 Wednesday, October 29, 2003 12:08 PM Autodesk Inventor® 8 Autodesk, Inc. 111 McInnis Parkway San Rafael, CA 94903, USA Tel.: +1/415-507 5000 Fax: +1/415-507 5100 Autodesk (Europe) S.A. 20, route de Pré-Bois Case Postale 1894 CH-1215 Geneva 15 Switzerland Tel.: +41/22-929 75 00 Fax: +41/22-929 75 01 Autodesk Asia PTE Ltd. 391B Orchard Road #12-06 Ngee Ann City, Tower B Singapore 238874 Singapore Tel.
INV8_TD_Book5.book Page 1 Tuesday, October 28, 2003 10:51 AM © Copyright 2003 Autodesk, Inc. All Rights Reserved This publication, or parts thereof, may not be reproduced in any form, by any method, for any purpose. AUTODESK, INC., MAKES NO WARRANTY, EITHER EXPRESSED OR IMPLIED, INCLUDING BUT NOT LIMITED TO ANY IMPLIED WARRANTIES OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE REGARDING THESE MATERIALS, AND MAKES SUCH MATERIALS AVAILABLE SOLELY ON AN “AS-IS” BASIS. IN NO EVENT SHALL AUTODESK, INC.
INV8_TD_Book5.
INV8_TD_Book5.
INV8_TD_Book5.book Page 1 Tuesday, October 28, 2003 10:51 AM Dear Design Professional, Welcome to the Autodesk Inventor® 8 Hands-on Test Drive! You are about to see why Autodesk Inventor software is the best choice for 3D mechanical engineering and design. This test drive demonstrates how Autodesk Inventor accelerates and simplifies your design process while extending your design capabilities.
INV8_TD_Book5.
INV8_TD_Main_46.fm Page 3 Thursday, October 30, 2003 3:12 PM Getting the Most from Your 30-Day Trial Version Getting the Most from Your 30-Day Trial Version System Requirements These are the recommended system requirements for the Autodesk Inventor 8 trial version: • Microsoft® Windows® XP Professional or Home Edition (SP1), Microsoft® Windows® 2000 Professional (SP2 or SP3) • Intel® Pentium III, Pentium 4, Xeon, or AMD Athlon™, 1 GHz or better processor (1.
INV8_TD_Book5.book Page 4 Tuesday, October 28, 2003 10:51 AM Getting the Most from Your 30-Day Trial Version Install Autodesk Inventor 8 30-Day Trial Version To install the Autodesk Inventor 8 30-day trial version: 1. In the Install screen, click the Install Autodesk Inventor 8 link and follow the instructions onscreen. 2. Click the Next button in the first dialog box. 3. Read the licensing agreement, confirm by clicking Accept, and then click Next. 4.
INV8_TD_Main_46.fm Page 5 Thursday, October 30, 2003 3:12 PM Getting the Most from Your 30-Day Trial Version Install Hands-on Test Drive Sample Files After installing the Autodesk Inventor trial version, you need to copy the sample files for the jogging stroller from the CD to your computer. To copy the sample, select the Install Sample Files link and follow the onscreen instructions. Note: We highly recommend installing the files in the folder C:\Inventor_r8_testdrive.
INV8_TD_Book5.
INV8_TD_Book5.book Page 7 Tuesday, October 28, 2003 10:51 AM Getting Started Getting Started To ensure the best possible performance and graphical representation of your work, we recommend that you use the following system settings. Tuning Your Graphics Settings To optimize the graphics settings on your system: 1. Right-click on the Windows desktop and choose Properties. 2. In the Display Settings dialog box, click the Settings tab. 3. Select True Color, and then click OK.
INV8_TD_Book5.book Page 8 Tuesday, October 28, 2003 10:51 AM Getting Started Help the Project Team Design a Jogging Stroller Before you start Autodesk Inventor software, we want to tell you about what you can learn from this booklet and invite you to join our jogging stroller project team. The finished jogging stroller is shown on the right. The first step is to design a clamp that can be used to adjust the height and inclination of the seat. The clamp assembly is also shown on the right.
INV8_TD_Book5.book Page 9 Tuesday, October 28, 2003 10:51 AM Getting Started Starting Autodesk Inventor To start Autodesk Inventor: 1. Double-click the Autodesk Inventor 8 icon on the desktop. application The Authorization dialog box is displayed with a reminder of the number of days remaining on your trial version of Autodesk Inventor. 2. Select the Run the product option and then click Next. The Getting Started page is displayed.
INV8_TD_Book5.book Page 10 Tuesday, October 28, 2003 10:51 AM Getting Started Starting with a Project Autodesk Inventor uses project files to organize and manage the multiple files associated with a design. For this jogging stroller design, a project file has been provided for you. To activate the project: 1. In the What to Do area of the Getting Started dialog box (left column), click Projects. 2. In the project window, right-click and choose Browse. 3.
INV8_TD_Book5.book Page 11 Tuesday, October 28, 2003 10:51 AM Getting Started Starting Your First Assembly First, you will create a new, empty assembly and then proceed to create or add components to that assembly as the design progresses. To create a new assembly using a standard template: 1. In the What to Do area of the Getting Started dialog box, click New. Another dialog box presents several template options for single parts, sheet metal parts, assemblies, drawings, and so forth. 2.
INV8_TD_Book5.book Page 12 Tuesday, October 28, 2003 10:51 AM Getting Started The Panel Bar The Panel bar offers specialized design tools that automatically change to reflect the environment you are working in. For example, when you create a new assembly, the Panel bar contains a set of tools for creating and placing components in the assembly. When you start a new component, the Panel bar contains a set of sketching tools to start sketching the component.
INV8_TD_Book5.book Page 13 Tuesday, October 28, 2003 10:51 AM Sketching Your First Part Sketching Your First Part The first part you are going to design is the upper clamp of the clamp assembly. The finished upper clamp is shown on the right. To create a new part in the assembly: 1. On the Panel bar, click the Create Component tool. 2. For the New File Name, type Clamp_top. 3. Leave all remaining parameters at the default values and click OK. To define the location of the component: 4.
INV8_TD_Book5.book Page 14 Tuesday, October 28, 2003 10:51 AM Sketching Your First Part To sketch the ellipse: 1. Move the cursor into the sketch area. The cursor now turns into a yellow point. 2. Move the cursor over the intersection of the axes as shown on the right. As you move the cursor close to the intersection of the two axes, notice that the yellow point is snapped and held at the point of intersection.
INV8_TD_Book5.book Page 15 Tuesday, October 28, 2003 10:51 AM Sketching Your First Part Determining the Size of Your Sketch To determine the size of your sketch, you will need to add some dimensions. Autodesk Inventor can generate many different dimension types — linear, angular, radial, diameter, and so forth —using one simple dimensioning tool. Adding Dimensions To add dimensions to your elliptical sketch: 1. On the Panel bar, scroll down and click the General Dimension tool. 2.
INV8_TD_Book5.book Page 16 Tuesday, October 28, 2003 10:51 AM Entering the Third Dimension 3. Repeat the previous steps for the vertical dimension using a value of 15.5. 4. To quit the General Dimension tool, press the Esc key or right-click in the graphics window and then choose Done. When you are finished defining the values of the dimension, your sketch should look like the image on the right.
INV8_TD_Book5.book Page 17 Tuesday, October 28, 2003 10:51 AM Entering the Third Dimension Finishing the Sketch To leave the sketch environment: • In the graphics window, right-click and then choose Finish Sketch. Notice that the grid is no longer displayed because it is only needed during sketching. Also notice on the Panel bar that the sketch commands have been replaced by the 3D modeling part feature tools.
INV8_TD_Book5.book Page 18 Tuesday, October 28, 2003 10:51 AM Entering the Third Dimension To create a parametric reference for the extrusion: 1. In the Extrude dialog box, double-click the current distance value (make sure that “mm” is also highlighted). 2. With the distance value highlighted, select the 15.5 dimension on the sketch. The parameter d1 now appears in the Extrude dialog box as the distance value. You have just created a link between the height of the ellipse and the extrusion distance.
INV8_TD_Main_45.fm Page 19 Wednesday, October 29, 2003 11:38 AM Entering the Third Dimension Changing the Color of Your Model You may also want to change the color of your model. To change the color: 1. On the right side of the Standard toolbar, click the down arrow next to As Material. 2. In the drop-down list of available colors and materials, select Metal-Steel (Polished).
INV8_TD_Book5.book Page 20 Tuesday, October 28, 2003 10:51 AM Adding Design Details Adding Design Details Next, you will add a bearing shell to your model. You will start by creating another sketch and then use that sketch to make another extrusion feature. Creating a Sketch Plane Using a Work Plane In the previous section you activated the assembly before saving it. To add features to your part, you must make the part active again. • In the Browser, double-click Clamp_top:1.
INV8_TD_Book5.book Page 21 Tuesday, October 28, 2003 10:51 AM Adding Design Details Referencing Existing Geometry The bearing shell must maintain a geometric relationship with the elliptical solid. You can easily use existing geometry by referencing existing dimensions or by projecting geometry onto the current sketch plane. 1. On the Panel bar, scroll down and click the Project Geometry tool. 2. In the graphics window, select the upper and lower elliptical edges of your 3D part.
INV8_TD_Book5.book Page 22 Tuesday, October 28, 2003 10:51 AM Adding Design Details Adding Constraints Constraints apply behavior to a specific object or create relationships between two objects. For example, a horizontal constraint can be applied to a line to ensure that line remains horizontal. This horizontal constraint can be applied automatically as you sketch the line, or manually to an existing line.
INV8_TD_Book5.book Page 23 Tuesday, October 28, 2003 10:51 AM Adding Design Details Checking the Sketch Visually You can visually check how complete your sketch is by interrogating the sketch geometry. To visually check your sketch: 1. Move the cursor over the objects in your sketch. The lines, circles, endpoints, and centerpoints are highlighted. 2. Move the cursor over the smaller circle, then select and drag the circle.
INV8_TD_Book5.book Page 24 Tuesday, October 28, 2003 10:51 AM Adding Design Details Drawing the Border Edge of the Bearing Shell Next, you will draw a line to bisect the circles. This line is later used to control the shape of the extrusion. To draw a line: 1. At the top of the Panel bar, click the Line tool. 2. Move the cursor over the intersection of the lower projected line and the left side of the outer circle (location 1 shown in the image). 3.
INV8_TD_Book5.book Page 25 Tuesday, October 28, 2003 10:51 AM Adding Design Details 2. Move the cursor over the upper half of the sketch, and when the upper semicircle is highlighted, click to select. 3. In the Extrude dialog box, type a distance of 55 mm, click the Centered option, ensure the Join then click OK. option is selected, and If you make an error, you can use the Undo Extrude feature again. tool to create the Your extrusion feature should appear as shown on the right.
INV8_TD_Book5.book Page 26 Tuesday, October 28, 2003 10:51 AM Adding Design Details 5. In the Extrude dialog box, click the Cut option, click the down arrow under Extents and select All, click the Centered option, and then click OK. Changing the Thickness of the Bearing Shell If you look closely at the model, you see that the bearing shell seems to be too thick. An ideal thickness would be 2 mm. The formula we used previously was d1-1.
INV8_TD_Book5.book Page 27 Tuesday, October 28, 2003 10:51 AM Adding Design Details Cleaning Up Before saving your work, you should clean up a few things. 1. To exit the sketch environment, in the graphics window, right-click and choose Finish Sketch. The sketch you shared is also visible. To turn off the display of this sketch: 2. In the Browser, between the Extrusion1 and Extrusion2 entries, right-click Sketch2 and choose Visibility to clear the check mark.
INV8_TD_Book5.book Page 28 Tuesday, October 28, 2003 10:51 AM Creating a Production Drawing Creating a Production Drawing Thus far we have created a 3D model, but what about creating technical drawings? With Autodesk Inventor software, you can derive drawings directly from your 3D models and your drawings are fully associative to those 3D models. This means that your drawings automatically update when your 3D designs change.
INV8_TD_Book5.book Page 29 Tuesday, October 28, 2003 10:51 AM Creating a Production Drawing Creating More Views You can easily create top, side, and isometric views directly from the front view. 1. On the Panel bar, click the Projected View tool. 2. Select the front view you just created, and then click to the right to define the location of the side view. A rectangular preview of the view is displayed. 3. Move the cursor below the front view and click to define the location for the top view. 4.
INV8_TD_Book5.book Page 30 Tuesday, October 28, 2003 10:51 AM Creating a Production Drawing Shading a View You can also enhance the appearance of your drawing views. To shade the isometric view: 1. Move the cursor over the isometric view (avoid placing the cursor over lines in the view), right-click and then choose Edit View. 2. In the Drawing View dialog box, click the Shaded button and then click OK. Adding Dimensions Next, you can add some dimensions.
INV8_TD_Book5.book Page 31 Tuesday, October 28, 2003 10:51 AM Creating a Production Drawing Inserting Centerlines Automatically Creating centerlines on your drawing views is simple with Autodesk Inventor. To generate centerlines automatically for the front view: 1. Move your cursor into the front view (lower-left view on your sheet), right-click, and then select Automated Centerlines.
INV8_TD_Book5.book Page 32 Tuesday, October 28, 2003 10:51 AM Creating a Production Drawing Removing Material from the Part To produce a clamping action when the two halves of the clamp are fastened together, you need to remove material from the bottom of the shell. You can do this by extruding a sketch and removing material from the part. First, you have to create a new sketch on the XY plane of the part. 1. In the Browser, click the plus (+) sign next to Origin directly below Clamp_top:1. 2.
INV8_TD_Book5.book Page 33 Tuesday, October 28, 2003 10:51 AM Creating a Production Drawing Changing the Outside Diameter of the Halfshell Next, you need to slightly reduce the outer diameter of the halfshell. However, a tangent constraint currently exists between the circular sketch of the halfshell and the upper face of the part. Before you can add a dimension to the outer circle in the sketch, you must first delete this tangent constraint.
INV8_TD_Book5.book Page 34 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly The Drawing Is Automatically Updated Autodesk Inventor always maintains full associativity between the model and the drawings. Since you have modified the model, the drawing automatically reflects those changes. This helps you avoid errors that would otherwise cost you time and money. To review and save the updated drawing: 1. From the Window menu, choose Clamp_top.idw.
INV8_TD_Book5.book Page 35 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly To create a new welded assembly component: 1. On the Panel bar, click the Create Component tool. 2. Important: In the Create In-Place Component dialog box, click the arrow next to Template and select Weldment.iam. 3. Type Clamp_welded.iam as the new file name and then click OK to close the dialog box.
INV8_TD_Book5.book Page 36 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Reusing Your Existing Design The shape of the lower halfshell is nearly identical to the upper clamp. Rather than designing the lower halfshell from scratch, with Autodesk Inventor you can derive the design of the lower halfshell from the upper clamp. Since you are deriving the design from another part, you do not need to use the default sketch that was automatically defined when you created this part.
INV8_TD_Book5.book Page 37 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Designing Fastening Holes Next, you need to design holes in the upper clamp. These holes, when combined with holes you will later create on the lower clamp, allow the two clamps to be fastened together. To make the upper clamp the active part and create a hole: 1. In the Browser, double-click Clamp_top:1. The upper clamp is now visible and the lower clamp is dimmed.
INV8_TD_Book5.book Page 38 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Filleting the Transition Next, you will fillet the transition between the halfshell and the elliptical body. Although this part requires only a simple constant fillet, Autodesk Inventor can create very complex fillets. 1. On the Panel bar, click the Fillet tool. 2. In the graphics window, select the two edges where the outer face of the halfshell intersects the vertical face of the elliptical body.
INV8_TD_Book5.book Page 39 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Mirroring the Tapped Hole The lower clamp also needs two holes to match the upper clamp. 1. On the Panel bar, click the Mirror Feature tool. 2. Select the tapped hole as the feature to be mirrored. 3. In the Mirror Pattern dialog box, click Mirror Plane. 4. In the Browser, next to Origin under the part Clamp_A:1, click YZ Plane. 5. In the Mirror Pattern dialog box, click OK to mirror the tapped hole.
INV8_TD_Book5.book Page 40 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Loft features require at least two sketches or boundaries. Your first sketch on this part will be based on the bottom face of the lower halfshell. 1. On the Panel bar, click the Project Geometry tool. 2. Select the elliptical edge on the bottom face of Clamp_A. 3. To quit the Project Geometry tool, in the graphics window, right-click and then choose Done. 4.
INV8_TD_Book5.book Page 41 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Sketching the Lower Contour Autodesk Inventor software offers many tools for establishing geometric links between objects. To ensure that the upper and lower contours remain aligned, you can use the Project Geometry tool to project the upper contour to the sketch plane as reference geometry.
INV8_TD_Book5.book Page 42 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Creating a Thin-Walled Part To reduce the weight and increase the strength of your lofted part, you need to hollow out the part using a constant wall thickness. You also want to keep both ends of the part open. 1. On the Panel bar, click the Shell tool. 2. To identify the faces to be removed, select the upper and lower planar faces of the part. 3. In the Shell dialog box, type 1.
INV8_TD_Book5.book Page 43 Tuesday, October 28, 2003 10:51 AM Working with Multiple Parts in an Assembly Making the Sketch Adaptive Next, you need to make this sketch adaptive. • In the Browser, right-click Sketch3 and choose Adaptive. The adaptivity icon is displayed next to Sketch3 in the Browser. Later in the design process when you define a geometric relationship between the geometry of this feature and geometry on the sheet metal part, the size of this cutout will adapt.
INV8_TD_Book5.book Page 44 Tuesday, October 28, 2003 10:51 AM Creating a Sheet Metal Design Creating a Sheet Metal Design Autodesk Inventor software has powerful sheet metal capabilities built right into the software. Sheet metal designs need to take into consideration a constant thickness, bend radii, relief sizes, and so forth. Autodesk Inventor enables you to easily manage all these sheet metal variables, and much more.
INV8_TD_Book5.book Page 45 Tuesday, October 28, 2003 10:51 AM Creating a Sheet Metal Design 3. On the Standard toolbar, click the Look At then select the circle. tool and Next, we need to append a line segment to the sketch. 1. On the Panel bar, click the Line tool. 2. Move the cursor over the lower-right quadrant of the circle. When the point is coincident with the circle and the icon is displayed, select the circle to create the first point of the line. 3. Move the cursor below the circle.
INV8_TD_Book5.book Page 46 Tuesday, October 28, 2003 10:51 AM Creating a Sheet Metal Design Mirroring and Editing Sketch Objects The Mirror tool can save you a lot of time when working with symmetrical parts. To mirror the lower line segment: 1. On the Panel bar, click the Mirror tool. 2. Select the lower line segment. 3. In the Mirror dialog box, click the Mirror Line option. 4. Select the construction line, and then in the Mirror dialog box, click Apply and then Done.
INV8_TD_Book5.book Page 47 Tuesday, October 28, 2003 10:51 AM Creating a Sheet Metal Design Creating a Sheet Metal Part from the Sketch Now, you create a sheet metal part using the open sketch. 1. On the Panel bar, click the title and select Sheet Metal Features. Note: If you do not see this menu option, perhaps you did not select the template Sheet Metal.ipt as described earlier. In this case, activate it from the Applications menu by selecting Sheet Metal. 2.
INV8_TD_Book5.book Page 48 Tuesday, October 28, 2003 10:51 AM Creating a Sheet Metal Design Creating an Adaptive Link Between Parts In the transitional part (Clamp_B), you intentionally underconstrained the cutout at the bottom of the part so that the diameter of the cutout could adapt to the outer diameter of the sheet metal part. Next, you will use an assembly constraint to place the sheet metal part at the center of the cutout and simultaneously establish a link between the two faces.
INV8_TD_Book5.book Page 49 Tuesday, October 28, 2003 10:51 AM Creating a Sheet Metal Design After performing these steps, the sheet metal part moves into the proper location and the lower cutout of the Clamp_B part adapts to the size of the outer face of the sheet metal part. Positioning Parts Accurately in an Assembly In the previous section you saw how to orient parts in an assembly with respect to one another.
INV8_TD_Book5.book Page 50 Tuesday, October 28, 2003 10:51 AM Designing Welded Assemblies Designing Welded Assemblies With Autodesk Inventor software, the process of creating a welded assembly is similar to the process in the real world. First, you start with an assembly of individual parts designed to their nominal size. Next, you can prepare those parts by removing material at the locations of the weld seams. Finally, you then weld parts together using different weld types.
INV8_TD_Book5.book Page 51 Tuesday, October 28, 2003 10:51 AM Designing Welded Assemblies 7. With the Arrow Side 1 selection button highlighted, select the edge where the previously created chamfers meet (the highlighted selection should display a completely closed loop). 8. In the Weld Feature dialog box, click Apply. The cosmetic weld is displayed on the model as an orange line with the weld symbol displayed to the side showing the weld seam type and size.
INV8_TD_Book5.book Page 52 Tuesday, October 28, 2003 10:51 AM Using iMate—Intelligent Mating of Components Using iMate—Intelligent Mating of Components Next, you will add a hole to the sheet metal part. After you add the hole, you will add intelligence to the hole so that other parts will constrain themselves to this hole automatically. You will also create a flat pattern that can be used to manufacture the sheet metal part. Adding a Hole 1.
INV8_TD_Book5.book Page 53 Tuesday, October 28, 2003 10:51 AM Using iMate—Intelligent Mating of Components To create the hole feature: 1. On the Panel bar, click the Hole tool. 2. In the Holes dialog box, select Through All for the termination, change the diameter to 7 mm, and then click OK. Creating a Flat Pattern Before you add intelligence to the hole, you should see how easily you can create a flat pattern of your sheet metal part.
INV8_TD_Book5.book Page 54 Tuesday, October 28, 2003 10:51 AM Using iParts—Intelligent Family of Parts Using iParts—Intelligent Family of Parts When you look closely at some parts in an assembly, many of these parts are nearly identical, differing only slightly in their size or the number of features. With Autodesk Inventor software, you can use iParts, or intelligent parts, to design the shape once, and then define many different versions using a spreadsheet.
INV8_TD_Book5.book Page 55 Tuesday, October 28, 2003 10:51 AM Using iParts—Intelligent Family of Parts Inserting the Fastener As an example of how iParts automate the design process, you will now place a fastener into the hole of the sheet metal part. This fastener was designed as an iPart with a variety of lengths and diameters. 1. On the Panel bar, click the Place Component tool. 2. In the Open dialog box, select the Use iMate check box in the lower-left corner. 3. Select the part Stud.
INV8_TD_Book5.book Page 56 Tuesday, October 28, 2003 10:51 AM Using Standard Parts To fully constrain the quick-action lever: 1. On the Panel bar, click the Place Constraint tool. 2. In the Place Constraint dialog box, click the Angle option. 3. In the graphics window, select the planar face of the plate on the quick-action lever, and then select the bottom edge of the sheet metal part as shown in the image to the right. 4. In the Place Constraint dialog box, click OK.
INV8_TD_Book5.book Page 57 Tuesday, October 28, 2003 10:51 AM Using Standard Parts Inserting Standard Parts into Your Assembly Now that you have identified the type of fastener that you want to use and have specified a size, you can insert the standard part into your assembly. 1. In the Browser, move the cursor over the preview of the bolt. As you move the cursor over the preview, the cursor image changes to an eye dropper. This is the symbol for the Autodesk i-drop® function. 2.
INV8_TD_Book5.book Page 58 Tuesday, October 28, 2003 10:51 AM Animating the Assembly Animating the Assembly In this section, you will see how you can use Autodesk Inventor 3D assembly designs for other applications such as creating assembly instructions, maintenance guides, marketing materials, and so forth. The Presentation Environment Now you are going to switch to a new working mode, the presentation environment.
INV8_TD_Book5.book Page 59 Tuesday, October 28, 2003 10:51 AM Animating the Assembly Your view of the assembly is changed to be consistent with the direction of the arrow you selected. 4. Select the green arrow shown in the image to the right. Your view of the assembly changes to a different isometric view. 5. Press the spacebar again to switch back to Orbit mode and then press the Esc key to quit.
INV8_TD_Book5.book Page 60 Tuesday, October 28, 2003 10:51 AM Animating the Assembly Repositioning the Upper Clamp Next, you will move the bolts and the upper halfshell part in a different direction. 1. With the Tweak Components dialog box still displayed, select the upper halfshell of the clamp (the bolts and the upper halfshell should be highlighted in blue). 2. In the Tweak Components dialog box, click the X option (or select the X arrow on the triad). 3. Drag the three parts to the left. 4.
INV8_TD_Book5.book Page 61 Tuesday, October 28, 2003 10:51 AM Reusing Your Existing 2D Design Data Reusing Your Existing 2D Design Data Designers have been using CAD systems for many years, which adds up to a great deal of existing drawings. Autodesk Inventor software makes digital data reuse fast and simple, and extends the value of your existing 2D designs.
INV8_TD_Book5.book Page 62 Tuesday, October 28, 2003 10:51 AM Reusing Your Existing 2D Design Data Selecting the Layers to Import Now you can identify which layers or geometry you want to import. The left side of the dialog box displays the layers that exist in the drawing file. Even though you can import the entire drawing, you may want to import only the contents you need. In this case, you need to import only the contours for the hub, which is on layer AM_1. In the AutoCAD OEM Viewer dialog box: 1.
INV8_TD_Book5.book Page 63 Tuesday, October 28, 2003 10:51 AM Reusing Your Existing 2D Design Data Moving into 3D Next, you start using the 2D data to create a 3D part. 1. On the Panel bar, click the Revolve tool. 2. In the graphics window, select the three closed profiles shown in the image to the right. Tip: If you accidentally select an incorrect closed profile, press and hold the Ctrl key and then select the closed profile you want to remove from the selection set. 3.
INV8_TD_Book5.book Page 64 Tuesday, October 28, 2003 10:51 AM Reusing Your Existing 2D Design Data Designing a Rib To create a rib feature using the shared sketch geometry: 1. On the Panel bar, click the Rib tool. 2. Select the line shown in the image to the right (the line lies in front of the rim). 3. In the Rib dialog box, click the Direction button. 4.
INV8_TD_Book5.book Page 65 Tuesday, October 28, 2003 10:51 AM Reusing Your Existing 2D Design Data Adding a Cutout to the Rim Next, you will add a cutout to the rim. Since the cutout must start on the inner face of the rim, you must create a new sketch. You can then copy the sketch geometry from the shared sketch to this new sketch. 1. Restore the Isometric View and then use the Zoom Window tool to zoom in on the rim. 2.
INV8_TD_Book5.book Page 66 Tuesday, October 28, 2003 10:51 AM Reusing Your Existing 2D Design Data Creating a Circular Pattern of the Cutout and Ribs The rim has a total of three cutouts and ribs. Rather than creating each of these separately, you can create a circular pattern of the existing features. 1. On the Panel bar, click the Circular Pattern tool. 2. To identify the features to pattern, in the Browser, click Rib1, Fillet2, Fillet3, and Extrusion1. 3.
INV8_TD_Book5.book Page 67 Tuesday, October 28, 2003 10:51 AM Creating an Assembly Drawing Creating an Assembly Drawing Next, you will create an assembly drawing of the entire jogging stroller. For the purposes of this test drive, we have provided you with the final assembly, including the finished clamp and the rim. Opening the Jogging Stroller Assembly The finished versions of the part and assembly files for the stroller are located in a separate folder on your system.
INV8_TD_Book5.book Page 68 Tuesday, October 28, 2003 10:51 AM Creating an Assembly Drawing Starting a New Drawing To start a new drawing for your assembly drawing: 1. On the Standard toolbar, click the New tool. 2. In the Open dialog box, select Standard.idw and then click Open. A new drawing with an A3 sheet size is created. Generating the First View The first drawing view you will create is an isometric view of the completed assembly. 1. On the Panel bar, click the Base View tool.
INV8_TD_Book5.book Page 69 Tuesday, October 28, 2003 10:51 AM Creating an Assembly Drawing Adding Balloons To identify all the parts in the detail view of the clamp, you can add balloons. Autodesk Inventor software automates the process of creating balloons on your assembly drawings. 1. Click the title of the Panel bar and then choose Drawing Annotation Panel. 2. On the Panel bar, click the down arrow Balloon next to the tool and then click the Balloon All tool. 3.
INV8_TD_Book5.book Page 70 Tuesday, October 28, 2003 10:51 AM Creating an Assembly Drawing Adding a Parts List Since Autodesk Inventor software manages information associated with parts and assemblies, you can easily create a parts list to accompany the balloons. To include a parts list with your balloons: 1. On the Panel bar, click the Parts List tool. 2. Click once on the detail view and then in the Parts List Item Numbering dialog box, click OK.
INV8_TD_Book5.book Page 71 Tuesday, October 28, 2003 10:51 AM Autodesk Manufacturing Solutions Portfolio Autodesk Manufacturing Solutions Portfolio Autodesk Inventor is one component in a comprehensive portfolio of integrated Autodesk products, partners, and services that enables you to use your design data across the entire manufacturing process.
INV8_TD_Book5.book Page 72 Tuesday, October 28, 2003 10:51 AM Autodesk Manufacturing Solutions Portfolio Create and Automate Complex Designs Using Autodesk Inventor Professional Autodesk Inventor Professional is 3D mechanical design software that combines the proven power of Autodesk Inventor with specialized design and validation technologies for mechanical and electro-mechanical engineers and designers.
INV8_TD_Book5.book Page 73 Tuesday, October 28, 2003 10:51 AM Autodesk Manufacturing Solutions Portfolio Manage Your Design Data Using Autodesk Vault Autodesk Vault is an engineering data management application for workgroups that is fully integrated with Autodesk Inventor and Autodesk Inventor Professional software solutions, at no additional cost.
INV8_TD_Book5.book Page 74 Tuesday, October 28, 2003 10:51 AM Autodesk Manufacturing Solutions Portfolio Sharing Your Design Data Using Autodesk Streamline Share your digital design data instantly, accurately, securely, and for less cost with Autodesk Streamline, an easyto-use hosted environment for sharing design and project data with anyone who needs it—anytime, anywhere.
INV8_TD_Book5.book Page 75 Tuesday, October 28, 2003 10:51 AM Conclusion Conclusion We hope you have enjoyed your 3D design experience. During this test drive, you had an opportunity to use Autodesk Inventor for • Sketching • 3D modeling • Adaptive design • Sheet metal design • Movement simulation • Part drawing creation • Assembly drawing creation • Reusing 2D AutoCAD drawings However, this only scratches the surface of the true capabilities of Autodesk Inventor.
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