Inventor 6a4r4t

BY CHRISTOPHER F. SIKORA

© Copyright 2015 Christopher Sikora

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This manual is for educational purposes only. It may be printed, but not resold for profit for its content. Inventor is a ed trademark of Autodesk Corporation. Inventor 2016 is a product name of Autodesk Corporation. ACIS is a ed trademark of Spatial Technology Inc. IGES™ Access Library is a trademark of IGES Data Analysis, Inc.

Other brand or product names are trademarks or ed trademarks of their respective holders.

The information discussed in this document is subject to change without notice and should not be considered commitments by Christopher F. Sikora. The software discussed in this document is furnished under a license and may be used or copied only in accordance with the of the manufactures license.

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Introduction to Inventor - IMT 110 Course Description: Intro to CIM 3 credit hours Exploration of the theory and application of Computer Integrated Manufacturing, beginning with CAD - solid modeling techniques for product design, CNC, and Computer Aided Manufacturing. Prerequisite: Intro to Engineering Drawings 101 or consent of instructor. (1 lecture hours, 2 lab hours) Course Objectives: Provide the student with the knowledge and practical experience in the areas of 3D CAD modeling of parts, assemblies, and the creation of mechanical drawings from the models. Textbook & Software Inventor Basics (pdf. provided) Instructional videos of lectures are available on YouTube channel: YouTube Link: Vertanux1 Web Page Link: www.vertanux1.com Software Page Link: Inventor Professional 2016 Software NOTE: When setting up an to software you must use your student .edu email address.

Evaluation Scale: A

90% to 100%

B

80% to 89%

C

70% to 79%

D

60% to 69%

F

Below 60%

Points: Labs

300 pts

Mid Term

300 pts

Final

300 pts

Participation/Attendance

100 pts

Total

1000 pts

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General Course Outline Date

Week Topic

8/20

1.

E1 - Introduction to CIM and Inventor CAD Interface Lecture CAD/CAE/CAM Theory

2.

E2 - Revolved Features and Mirroring

3.

E3 - Part Modeling Secondary Features. Fillets, Chamfers, Draft, Patterns, Mirroring.

4.

E4 - Sweeps, and Circular Patterns (Review for Quiz 1)

5.

Q1 - Modeling Quiz and CIM istration

6.

E5 - Building Assemblies (Bottom-Up method “BU”)

7.

E6 - Creating Drawings. Review for Mid Term

8.

Mid Term Exam

9.

E7 - Computer Aided Engineering (CAE)

10.

E8 – Lofts (Boat)

11.

E9 - Computer Aided Manufacturing (CAM)

12.

E10 - Advanced Freeform (G2) bottle

13.

Design Project, Sketching, Modeling, & Rapid Prototyping

14.

Design Project, Intro to PowerPoint

15.

Lab time to complete Design project, Presentations

16.

Presentations/Design projects and Exercises 1 thru 10 due

10/8

12/10

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Chapters 1.

Introduction to the Interface Modeling Theory - Sketching and Base Feature Geometry Creation.

2.

Part Modeling Revolved Method

3.

Secondary Feature Modeling (Draft, Offsetting Entities, Filleting)

4.

Advanced part Modeling (Sweeps, and Circular Patterns)

5.

Bottom-Up Assembly Modeling

6.

Creating Drawings

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7.

CAE (Computer Aided Engineering)

8.

Lofting

9.

Inventor to Mastercam

10. Advanced Freeform Modeling

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Introduction to Inventor Professional

2016 Interface

Icons Quick Launch Options

Browser/Feature Manager

View port

Mouse Buttons Left Button - Most commonly used for selecting objects on the screen or sketching. Right Button – Used for activating pop-up menu items, typically used when editing. Center Button – (option) Used for model Pan, Rotate when holding Shift key. Center Scroll Wheel – (option) same as Center Button when depressed, only it activates Zoom feature when scrolling wheel.

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Options menu “The hearts of Inventor”… Selecting the Grid Icon opens the Options Menu or the Tools/Options pull down can be used.

Application Options – (Global Settings) are setting that affect all documents. Location: Upper Left corner icon with the big yellow “I”, then find “Options” at the bottom center of the list or Tools>Application Options.  Screen Background Color  Performance Settings  Interface Preferences

Document Settings – (Individual Document Settings) are setting that adjust only the currently active document. Location: While in a part (.ipt) or an assembly (.iam) document got to Tools>Document Settings.  Part Color  Units  Standards

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Sketching (2D tools)

Where do you start a sketch? Sketches can be created on any Plane or Planar Face or Surface. Inventor provides you with three planes centralized at the Origin (your zero marker in space) NOTE: Planes can also be created and will be discussed in more detail in the future.

To start a sketch Pre-select the plane or face you desire to sketch on and then select the quick launch Sketch Icon that appears automatically. NOTE: You can select the planes from the “Browser - Feature Manager”.

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Controlling your geometry…

Inventor uses two methods for constraining geometric entities. Relations and Dimensions Relations can be referred to as common elements of geometry such as Tangency, Parallelism, and Concentricity. These elements can be added to geometric entities automatically or manually during the design process.

Here is an example of adding a relationship between two geometric entities.

By selecting both entities Inventor will automatically activate the properties menu on the right side of the screen enabling the to input the desired relation.

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Cautious sketching can save time. Here are some tips to avoid modeling errors.

This is acceptable because it is a closed contour. Use the “Trim” tool to cut and extend.

This is unacceptable because it has untrimmed geometry.

This is unacceptable because it has multiple contours share a common entity.

There are 3 primary file types in Inventor, which include… 1. Part (.ipt) Single part or volume. 2. Assembly (.iam) Multiple parts in one file assembled. 3. Drawing (.idw) The 2D layout containing views, dimensions, and annotations.

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Controlling your geometry with dimensions…

Dimensioning this way will enable the length of the bracket to change but the holes will always remain positioned to 1.5” off each side.

Dimensioning this way will enable the length of the bracket to change but the holes will always remain positioned to the left side.

Features (3D tools)

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Solid Modeling Basics Layer Cake method Extruded Boss/Base (Creates/Adds material) Extruded Cut (Removes material) Ingredients:  Profile

Revolve method Revolve Boss/Base (Creates/Adds material) Revolve Cut (Removes material) Ingredients:  Profile  Center Line (Note: The profile cannot cross over the center line!)

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EXERCISE 1 Introduction to basic part modeling Base Extrude Features create a 3D solid representation by extruding a 2 dimensional profile of the entity. Objective: Create a solid model.

This will create a hole.

This will fail to extrude.

1. Start a new “part” file.

5. Select to add the dimensions.

3. Select the Rectangle tool. 2. Select the Sketch icon.

5. Select Finish Sketch.

4. Click and drag across.

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7. Select Extrude

9. Hit “OK” to apply.

8. Set to Blind @ .5”.

10. To sketch the next feature select the front face of the model and then select the “Create Sketch” quick launch icon.

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11. Use the rectangle tool to sketch from the lower left corner, approximately 1.5 inches to the right edge, when you see the little constraint symbol appear hit “tab” to edit the vertical dimension and insert 1.5”. Hit “Finish Sketch”.

12. Go to the Model tab, and then select “Extrude”. 13. Insert .5” depth. Hit the green check mark to apply.

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Adding the hole

1. Select this face and start a sketch.

2. Select the circle icon, and begin by locating the center of the circle, LMB (left mouse button) click, and drag out the circle by LMB clicking again.

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3. Using “Dimension” add the shown dimensions.

4. Select the Extrude icon.

5. Select the “Cut” option.

5. Select the “All” option.

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Go to the

icon and save-as “E1”

FINISHED Now try LAB1… NOTE: Patterns/Arrays and Mirroring will be covered in the next three chapters. Please try to model LAB 1 without using them. It’s good practice to just dimension and sketch all geometry when first starting out learning this software.

Please understand that I don’t want to overwhelm you with too much information the first day. It is my goal to help you succeed, not to fail.

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EXERCISE 2 Revolved Features Revolved Feature - creates features that add or remove material by revolving one or more profiles around a centerline. The feature can be a solid, a thin feature, or a surface. Tips… Profile Centerline, Edge, or Axis of Revolution

The profile should never cross over the centerline, nor should there be profiles on both sides of the centerline.

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1. Create a new part file (E2) and then start to sketch horizontal and vertical centerlines.

2. Sketch the following. Ctrl select the profile and the horizontal centerline, then using the “Mirror” tool to create a ¼ of the geometry and then mirror it to the other side. Make sure you finish adding the dimensions.

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3. Select the Revolve feature icon.

Then select the axis/centerline.

4. Select the top and bottom edges and add a .100” fillets.

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EXERCISE 3 Secondary Feature Modeling 1.

Start a new part file and sketch the geometry as show below.

2.

Extrude. Select Mid-Plane, 1” and add 7 of draft located in the “More” tab.

7 degrees

1”

Mid-Plane

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3.

Select the front face of the model and start a sketch on it.

4.

Use the “Offset” icon to offset sketch geometry .125” from the outside edges..

5.

Cut Extrude at .125” deep.

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6.

Select the base of the pocket and start a sketch on it.

7. Go “normal to” and sketch the following. Draw two circles on the center points of the outside arcs. Use the trim tool to remove intersections.

9. Extrude cut .75” deep.

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1. Select the base of the new pocket and start a sketch on it.

11.

Sketch the following, and extrude cut “Through-all”.

12.

Go to the Plane icon and select Offset from XZ plane in the feature tree, then click on the dimension to change it to -4.00”.

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13.

Start a sketch on “Work Plane 1” and draw a .5” dia. circle centered on the origin.

14.

Extrude and use the “To next” option.

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15.

16.

Start a sketch on the “Front” plane and sketch the following rectangle. Use a centerline with a midpoint relationship to center the rectangle to the origin.

Extrude boss using the mid-plane option and .750 thick with 7° draft.

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17. Using the fillet tool select the following edges and put a .125” radius on them.

18. Add additional fillets of .06” on the following edges.

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EXERCISE 4 Sweeps, Circular Arrays and Secondary Feature Modeling 1.

Sketch the geometry as show below on the “Front” plane.

2. Select Revolve.

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3. Select the “XY – aka: Front” plane and start a sketch on it. Rebuild after completion.

4. Create a plane using the “Plane” tool located under “Parallel to Plane through Point” Select “Finish Sketch”. Note: The 2 ingredients for creating a Parallel plane to a curve are the YZ plane and the end Point of the curve you just completed in the last section.

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5. In the “Left” view orientation select the new plane and RMB click on the end of the curve, select Project Geometry.

6. Sketch the following using center point arc and lines, and insert relations and dimensions as shown.

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7. Creating a Sweep: Select the Sweep Icon. Then select the Path and Profile.

8. Add .188” Fillets on the bottom edges of the spoke.

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9. Add .25” fillets to the intersection of the Spoke and Center.

Creating the Circular Pattern/Array

10. Select the spoke feature then select the Circular Pattern Icon. Then select the Rotation Axis icon and the actual cylinder face located at the center and the Spoke. Enter 3 for the number of spokes. Note: be sure to select the fillets as well, or they will not show up on the instances.

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2. Select the “XY” plane and start a sketch on it. Draw the following and don’t forget the Centerline.

3. Select the Boss-Revolve Icon, and revolve 360 “One-Direction”.

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4. Add .25” fillets around the intersections of the handle and spokes”.

5. You are finished.

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Using the Hole Wizard

1. 2. 3. 4.

Select the Hole icon Select the Concentric option if on a circular face. Select the face where the hole is to be placed Specify the size and type

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H

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EXERCISE 5 Bottom-Up Assembly Creation 1.

2.

Go to “File/New and select the “Standard.iam” (Assembly) template”.

Assemblies Toolbar.

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3.

To insert a part into the assembly go to “Place”.

4.

Search for the “Sheet Metal Bracket” in the Exercise 5 folder provided. Then move the pointer to the viewport and click the LMB to insert. Parts available on www.vertanux1.com

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5.

Go thru the insert steps again to bring in the “Yoke Male”, drop it to the left of the “Sheet Metal Bracket”.

6.

Select the “Constraint” icon and then select “Insert” option. Next, select the side face of the boss sticking out at the top of the Yoke. Then select the inside face of the hole on the bracket. Select Apply.

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7.

8.

Select the concentric option and apply. The part should now move into place.

Insert the “Spider” part next and mate it between the legs on the yoke, you may need to select mate alignment or Flush in order to rotate the part 180 degrees.

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9.

Use a concentric mate to align the center hole with the holes on the yoke.

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10.

Attach the remainder of the components.

11.

After completion you should be able to LMB click on the handle to dynamically rotate the assembly.

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EXERCISE 6 Fundamental 2D Drawing Creation 1.

Open the “E6” part file.

2.

IPro/New/Drawing

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3.

One method of inserting a part (E6) into a drawing is to first open the desired part file.

4.

Selecting a different Template: Notice the options for Sheet Format/Size will pop up. Select A- Landscape and hit New Sheet.

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5.

6.

Inserting a View: You should now see the paper border and the front view image. Double click on the image to access the “Drawing View” options. Change Scale to 1:2.

Select “Projection”, then select the “Front” view, move your pointer up and click to drop a top view, then right and click, and corner right and click. Right Mouse Button click to create.

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7.

Section Views: Select the “Section View” icon and then locate the left side quadrant edge of the top view and click on the edge. While a short distance away from ing the edge LMB click and drag a line horizontally through the entire view. (Don’t stop in the middle).

8.

Once through release the LMB and you should be able to now drag off a section view and drop it just above the “Top” view by LMB clicking again.

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9.

Detail Views: Select the “Detail View” icon. The circle tool is automatically activated so then you can draw a circle surrounding the region you wish to create a detail view from.

10.

Move the view to the desired location and LMB click to release/drop it.

Note: the view scale can be changed by simply double clicking on the “scale” text and typing in a new value, and the position and diameter of the circle can be changed dynamically by LMB clicking and dragging its center or diameter.

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Auxiliary Views: Can be created by selecting an edge of the part and then select the Auxiliary view icon.

11.

Then drag out the view and LMB click to drop it into position.

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12.

Editing the Sheet and Sheet Format: The “Sheet” is the transparent top level containing the model views, dimension and notes. The “Sheet Format” is the lower level that contains the border, title block, and notes.

13.

RMB click on the “SHEET1” tab located at the bottom left corner of the screen, and select “edit sheet format”.

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14.

Dimensions and Annotations: To add independent and non-parametric dimensions you can select the “Dimension” icon. Then just add dimensions the way you would in the sketcher. Otherwise you can use the “Retrieve” option in the “Annotate” tab.

15.

The “Retrieve” tool gives you access to dimensions and annotations added to the model during its construction by the designer. These annotations can be inserted automatically into the drawing. These are true, editable, parametric dimensions. Try using some of the other annotations like Note, Surface Finish, Welds, and GD&T.

16.

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IMT 110 Mid-Term Exam 1. Model the BOTTLE drawing “A”. (50 Points)

2. Model the CAP drawing “B”. (50 Points)

3. Create the BOTTLE assembly and attach the cap to the bottle. (100 Points)

4. Recreate the MEDICINE BOTTLE assembly drawing “C”. (100 Points) Note: Do not forget to insert your name on the drawing. Print out the drawing and turn in.

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EXERCISE 7 Introduction to Computer Aided Engineering (CAE) Stess Analysis FEA can be very useful for testing failure of a part. 1.

Go to file new and select “part” from the options.

1000 psi

2.

Objective: Create bottle opener. Perform FEA analysis to test for failure.

FIXED FACE

Select the “Material” option on the top options bar next to the beach ball icon, Locate and select ABS Plastic from the list.

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3.

Select the front plane and use the line tool to sketch the geometry called out on the attached drawings.

4. Extrude .400” depth. Add .3” and .1” fillets. Select ABS Plastic (top options bar)

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5. Go to “Environments/Stress Analysis”, Create Simulation.

6. Select “OK”.

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5. Select “Fixed”.

6. Select the underside face of the bottle opener, where the bottle cap would the opener. This is considered the fixed face because it rests on the cap. Select “OK”.

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7. Select “Force”, elect the underside face of the model. Enter 40 lbs.

8. Select “Simulate”, and select “Run”.

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9. At the next screen hit “Next” and “Run” to begin the simulation.

10. Select “Animate” Hit the “play” icon.

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EXERCISE 7b Computer Aided Engineering Case Study PROJECT: Monitor Wall Mounting Bracket

InLite®, a major manufacturer of Video and Television mounting components has commissioned the analysis of their latest polymer (Plastic) based LED Television mounting bracket. Because LED (Light Emitting Diode) technology enables televisions and monitors to be nearly half the weight of traditional LCD (liquid crystal) or Plasma displays.

Your task is to analyze the design to accommodate the weight of a typical 37” LED display. Write a minimum two page report on your findings with visuals (FOS2 & Stress plot).

70lbs PSI

FIXED SURFACE PSI

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Creating an Analysis Report

It’s important to include relevant data extracted from the analysis. And also be able to explain the purpose and noted critical regions with logic behind their selection. Here is a partial sample of a report.

Items to include in a report:

Cover page 

Name



Project name



Date

Purpose Page 

Define the purpose



Images with highlighted regions analyzed – Explain you decisioning.



Material

Each analyis should have it’s own page or pages with images and coplete descriptions of the results.

Bad reports typically lack explainations, and have little content. Good report is to the point with clearly labeled explainations. Images play a large role in analyis thus you should try and include all relavent and descriptive image results.

Liability When writing a report be careful to avoid putting yourself in a difficult situation. FEA analysis is not an insurance policy and it’s results can be flawed.

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PHONE BEZEL STUDY March 8, 2010 HEALY CORPORATION BY: CHRISTPHER F. SIKORA

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Purpose The purpose of this study was to evaluate the structural integrity of the engineered design, as well as to determine the elements of a controlled failure. Preliminary studies indicated there are two assemblies (Handset and Phone Bezel) with a total of 3 regions, which required advanced analysis. FEA-Finite Element Analysis software was used to identify undesirable feature characteristics through computer simulation. This document presents chronologically the process of identification, correction and optimization of engineered features. Material: Nylon 101 (MPa Threshold 45 < or =) ANALYIS B TOP BEZEL CORNER RISK OF FAILURE

ANALYSIS A BEZEL CORNER RISK OF FAILURE

ANALYIS C HANDSET CORNER

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ANALYSIS – A BEZEL 5ft. Drop Test March 10, 2010 Purpose: The Phone Bezel lower left corner may require additional reinforcement to prevent failure or cracking. During analysis we discovered the corner endures an MPa of 46.8 which exceeds the given threshold just slightly. We suggest that reinforcement of the interior corner ribs be adjusted and thickened from .06” to .100”. (see Fig.1)

FLOOR

ANALYIS A

IMPACT

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Reinforcement Region 1 By increasing the rib thickness to .100 the phone should be able to endure the projected forces.

Figure 1: Questionable region

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EXERCISE 8 Lofting Lofting creates a feature by making transitions between profiles. A loft can be a base, boss, cut, or surface. Objective: Create a boat hull by lofting multiple section profiles.

1.

Create four (4) planes beginning from the “XY Front” plane and offset from each other as shown. Plane 1 – 6.00” Plane 2 – 8.00” Plane 3 – 1.00”

2.

Sketch 1 on the “XY Front” plane should look like this… use the Spline tool.

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3.

Sketch 2 on “Plane 1” should look like this…

4.

Sketch 3 on “Plane 2” should look like this…

5.

Sketch 4 on “Plane 3” should point at the origin.

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7.

Loft: Exit any sketches and select Loft.

8.

Profiles: Select the four profiles in order from back to front of boat.

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9.

Use the Mirror feature and select the flat side face as the plane to mirror from.

10.

Select the hull as the feature and hit OK to apply.

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11.

You are finished with the boat Hull.

12.

(Optional) Now dress it up for the contest…

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EXERCISE 9 Basic Machined part modeling for Mastercam

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1. Draw on the XY plane and extrude the following 1” thick.

2. Sketch the circles and extrude them.

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3. Sketch the following and extrude cut it.

4. Extrue cut .5” deep.

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5. Add .25” fillets in the corners of the square cutout.

6. Save the part as E9. 7. Start Matercam and import the Autodesk Inventor E9.ipt. be sure to set your “Files of type” filter to Autodesk Inventor files.

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8. Once the file is impoted turn on shaded mode.

9. Select stock setup from the feature tree.

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10. Select all solids.

11. Selecting Material: Go to the Tool Settings tab and select Mill Library at the bottom and find Aluminum 6061.

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12. Select Properties and Mill Default in the Feature tree, and select Drill. Note: you can select under Machine Type your specific Postprocessor for the CNC you currently are using.

13. Select the bottom floor surfaces for the drill. Select the green checkbox.

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14. Select the Tool option, and then select the Library Tool

15. Select a 1/2” (#6) DIA. Drill. Hit the two green check boxes.

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16. Repeat the same steps to add a ¼” DIA (#5) drill for the second hole. Hit the two green check boxes.

17. Pockets: Select the Pocket tool

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18. Select solids, and then select the floor of each pocket. Select the green check box.

19. Select Tool, Select Tool. Select the ½” FLA (FLAT) (#239). Select the green check box.

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20. Select Roughing, and Constant overlap Spiral. Hit the green check box.

21. Select Machine Group 1 from the top of the feature tree, then select the Backplot icon.

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22. Adjust the setting as seen below and select the Machine icon to begin the toolpath simulation.

23. Watch the simulation.

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24. G-Code Program Output – Select Post to have Mastercam generate the program.

Finished

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EXERCISE 10 Lofting with Guide Curves 1. Sketch the geometry as show below on the “XY-front” plane. Rebuild. (5 spline points) Use ordinate dimensions for simplicity.

2.

Select Offset plane and offset a datum plane 8” from the XY-front plane.

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3.

Sketch the following on Plane 1. (5 spline points)

4.

Start a sketch on the top plane, and draw the following. (3 spline points)

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5.

Start a new sketch on the top plane and draw the following. (5 spline points)

6.

Loft

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7.

Loft completed.

8.

Creating G2 Curvature Continuous Fillets. Select the bottom edge of the bottle. Select the fillets icon. Input .250” radius and check Smooth G2.

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What are G2 Curvature Continuous fillets? Use Smooth G2 fillets to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross-section as opposed to a circular crosssection. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary. (Source: SolidWorks help)

9.

Select the back flat face and go to Insert/Mirror all.

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10.

Insert the neck of the bottle as shown below.

11.

Creating a Thread - Select the side face of the neck and go to the thread tool to add a cosmetic thread to the neck.

12.

Complete the other side the same way. Add additional features to finish bottle. Shell at .050”.

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