Chapter 6 Creating and Documenting Assemblies

After completing this chapter, you will be able to perform the following: – Understand the assembly options – Place components into an assembly – Create components and assemblies – Create subassemblies – Constrain components together using assembly constraints – Edit assembly constraints – Pattern components in an assembly – Check parts in an assembly for interference – Drive constraints – Create a presentation file – Manipulate and edit the Bill of Materials (BOM) – Create individual and automatic balloons – Create and perform edits on a Parts List of an assembly Chapter 6 - Objectives

Creating Assemblies New Assembly Files –.IAM Extension What To Do –Quick Access toolbar - New icon – Down Arrow –Quick Access toolbar - New icon –Inventor Application Menu - New icon

Creating Assemblies Assembly Options –Tools tab > Application Options > Assembly tab

Creating Assemblies Placing Components –Components are created in their individual files –Place Component tool –Shortcut key “P”

Creating Parts in Place Create a Part in the Context of an Assembly –Initial Sketch Creation Face of an existing assembly component Work Plane –Automatically constrain the sketch plane to the selected face or work plane Creates a Flush constraint between the sketch and the selected face or plane

Creating Parts in Place Create a Part in the Context of an Assembly –After the base feature is created Create additional features based on geometry from another part in the assembly an adaptive work plane is created. The adaptive work plane moves as necessary to reflect changes in the component that it is based upon –The sketch moves with the plane –Features based on the sketch adapt to match its new position

Creating Assemblies Assembly Browser –Part Occurrence –Assembly Constraints –Subassembly Occurrence

Creating Assemblies Occurrence –Copy of existing components Copy/Paste Ctrl Select Multiple Files Place Component Drag & Drop –Any change to original updates all occurrences Save Copy As… to create a copy that is not linked to original

The Assembly Capacity Meter Number of occurrences in active assembly Number of open files Memory (RAM) used (32 bit operating systems only) Application Option

Editing a Component in Place Active Component – Available for edit –Double-click in the graphics area –Double-click file name/icon in the Browser –Right-click in the Browser > Edit –Return Commands

Opening and Editing Components Open or Edit –Access via Browser Graphics window

Creating Assemblies Grounded Component –The Component will not move All Degrees Of Freedom are removed When constraining, components move to a Grounded or constrained component –Any number of components can be grounded

Degrees of Freedom (DOF) Assembly Constraints –Relationships between components i.e. Bolt and a Hole –Degree of Freedom Constraints reduce the number of Degrees of Freedom –6 total (3-translational & 3-rotational) –View tab > Visibility panel > Degrees of Freedom –Component Properties > Occurrence tab Degree of Freedom Analysis

Assembly Constraints Constraints –Placing Constraints Constraint command or shortcut key “C” Place Constraint dialog box –Limits Specify the distance or rotation that a component can deviate from an exact location

Assembly Constraints Constraint Types – Assembly tab –Mate Plane, Line, or Point –Assembles two components so that the surface normal on the selected planes are opposite each other –Assembles the edges of lines –Assembles two points together –Flush Solution Aligns two components so the selected planes face the same direction (surface normal point in the same direction)

Assembly Constraints Constraints –Constraint Types – Assembly tab Angle –Specify the degrees between the selected planes or use an Explicit Reference Vector

Assembly Constraints Constraints –Constraint Types – Assembly tab Tangent –Defines a tangent relationship between planes, cylinders, spheres, cones, and ruled splines –At least one selected face must be a curve –Inside/Outside Solutions

Assembly Constraints Constraints –Constraint Types – Assembly tab Insert –Two circular edges –Centerlines are aligned & mate constraint is applied to the planes defined by the circular edges. –5 DOF are removed with an insert constraint

Assembly Constraints Constraints – Constraint Types – Motion tab Animation the motion of gears pulleys, rack and pinions, etc. –You can drive one component and cause others to move accordingly Motion constraints are secondary constraints –They do not maintain positional relationships between components Recommended: fully constrain components before applying motion constraints, then suppress the constraints restricting motion –Rotation Define a component that will rotate in relation to another component Specify a ratio for the rotation between the two components Forward & Backward solution types

Assembly Constraints Constraints –Constraint Types – Motion tab Rotation-Translation –Define rotation relative to translation of a second component

Assembly Constraints Constraints –Constraint Types – Transitional tab Transitional –Specifies a transitional relationship between a cylindrical part face and a contiguous set of faces on another part

Assembly Constraints Constraints –Constraint Types – Constraint Set Constrain two UCSs

Select Geometry Select Other command –Set time in Application Options > General tab –Click arrows or scroll the wheel

Direct Select - Assembly Constraints Assemble command –Constraint is inferred from selected geometry –Use mini-toolbar to select specific options –The Assemble command moves the first component to the second

Assembly Constraints Constraints –ALT – drag a part to another part No Place Constraint dialog box Select correct area on the part to apply the constraint KeyConstraint Type M or 1Mate A or 2Angle T or 3Tangent I or 4Insert R or 5Rotation-Motion S or 6Rotation-Translation X or 8Transitional

Assembly Constraints Moving & Rotating Components –Move Component Tool Drag individual components in any linear direction in the viewing plane Temporarily suppresses assembly constraints on the component until the assembly is updated (constraints are then re-applied) –Rotate Component Tool After selected, the 3D rotate symbol appears Similar to the Move Component tool, Rotate Component temporarily suppresses any assembly constraints applied to the component

Assembly Constraints Editing Constraints –Two Methods via the Browser Double-click the constraint name Right-click the constraint name and click Edit, Suppress, or Delete –Edit - opens the Edit Constraint dialog box –Suppress – the assembly constraint is not applied –Delete – deletes the assembly constraint –Modify – change constraints value

Exercise 6-1 Assembling Parts

Assembly Constraints Browser Views –Assembly View Assembly constraint symbols nested below constrained components –Modeling View Assembly constraints are located in a Constraints folder

Find Other Half Find component that constraint is applied to Constraint Tooltips –List constraints and components

User-Defined Assembly Folders Organize components into folders Unlimited number of folders Add components to new folder Drag components into folders No affect on assembly constraints

Isolate Assembly Components Display selected components –Isolate Components and Edit Constraint Undo Isolate – return visibility of components before isolating

Assembly Constraints Isolate Constraint Errors –Alert Box If you try to place or edit an assembly constraint and it cannot be applied, an alert box is displayed explaining the problem. –Conflicting When assembly constraint conflicts with another one, a small yellow icon with an exclamation point is displayed in the Browser –Recover Displays the Design Doctor to walk you through the steps to fix the problem

Assembly Browser Commands Tools –In-Place Activation Double-click a subassembly or component occurrence in the Browser to activate it Right-click > Edit All components that are not active are shaded in the Browser

Assembly Browser Tools –Visibility Control Expand the Browser until the desired component occurrence is visible Right-click > Visibility

The Assembly Return Tool Return to subassembly Return to top level assembly

Adaptivity Definition –Allows the size of a part to be determined by setting up a relationship between the part and another part in the assembly Under-constrained sketches and features can adapt The adaptivity relationship is acquired by applying constraints between an adaptive sketch or feature and another part –The sketch cannot be fully constrained –A part can only be adaptive in one assembly at a time –Only one occurrence of a part can be adaptive – other occurrences reflect the size of the adaptive part –Example Diameter of a pin from the size of a hole or vice-versa

Adaptivity Example –The rectangular sketch is not dimensioned along its length –The extruded feature is defined as adaptive

Adaptivity Example –Parts are placed, constraints applied between the two plates (flush between the faces on the ends of the plates)

Exercise 6-2 Designing Parts in the Assembly Context

Pattern Components –Rectangular –Circular –Based on Feature Pattern –Suppress Elements –Pattern Assemblies –Replace Components

Exercise 6-3 Patterning Components

Minimum Distance Command In an assembly measure distances between –Components –Parts –Faces and Edges

Analysis Tools Center of Gravity –View tab > Visibility panel > Center of Gravity Displays Gray when the properties are out of date Hover the cursor over the origin of the symbol to display the COG coordinates Measure to Center of Gravity’s center point, planes and axes

Analysis Tools Interference Checking –Analysis tab > Interference Panel > Analyze Interference Define Set # 1 – select components that define set 1 Define Set # 2 – select components that define set 2 Or place all components in Set # 1

Exercise 6-4 Analyzing an Assembly

Driving Constraints Drive Constraint tool –Simulate motion Right-click on a constraint in the Browser > Drive Constraint

Driving Constraints Drive Constraint tool –Assembly Constraints –Record –Drive Adaptivity –Collision Detection

Exercise 6-5 Driving Constraints

Presentation Files.IPN Extension –Exploded Views –Hide specific components –Create animations of assembly and disassembly of components –Work Plane Associated with the assembly file –Changes made to the assembly are reflected in the presentation file

Presentation Files Presentation tab Create ViewCreates views of the assembly Tweak Components Moves and/or rotates parts in the view Precise View Rotation Rotates the view by a specified angle direction using a dialog box AnimateCreates an animation of the assembly – AVI file can be output

Presentation Files Creating Presentation Views –Create a presentation view Create View tool Adds a presentation view to the file and the Browser

Presentation Files Creating Presentation Views –Tweaking Components Tweak Component Dialog Box –Manual Tweaks

Presentation Files Creating Presentation Views –Tweaking Components Moves or Rotates components a specified distance or angle Auto Explode –Extends all tweaks the same distance

Presentation Files Creating Presentation Views –Animation Animate Tool –Controls for playback –Record to AVI or WMV file

Presentation Files Creating Presentation Views –Animation Animate Tool > More button –Changing the Animation Sequence –Move Up / Down –Group / Ungroup

Exercise 6-6 Creating Presentation Views

Creating Drawing Views (Assemblies & Presentations) Base View –Base View tool –IAM and IPN files

Creating Drawing Views - BOM Editor Edit item number, quantity, part number, description, vendor, etc. The BOM is also associative to parts and assemblies Edit like a spreadsheet Highlight components

EXERCISE 6-7 Editing the BOM

Creating Drawing Views (Assemblies & Presentations) Balloons –Balloon tools Balloon - Single Components Auto balloon – Selected Components

Creating Drawing Views (Assemblies & Presentations) Balloons –Editing Right-click a balloon > Edit Balloon Edit Balloon dialog box –Balloon Type –Balloon Value

Creating Drawing Views (Assemblies & Presentations) Parts List –Parts List tool Select a view Enter options in the Parts List dialog

Creating Drawing Views (Assemblies & Presentations) Bill of Materials dialog box Edit the assembly BOM All changes are saved in the assembly and corresponding component files

Creating Drawing Views (Assemblies & Presentations) Parts Lists –Editing Right-click and click Edit Parts List

Exercise 6-8 Creating Assembly Drawings

Applying Your Skills Skill Exercise 6-1Skill Exercise 6-2

Checking Your Skills 1.True False The only way to create an assembly is by placing existing parts into it. 2.Explain how to create a component in the context of an assembly. 3.True False An occurrence is a new copy of an existing component. 4.True False Only one component can be grounded in an assembly. 5.True False Autodesk Inventor does not require components in an assembly to be fully constrained. 6.True False A sketch must be fully constrained to adapt. 7.What is the purpose of creating a presentation file? 8.True False Balloons can only be placed in a drawing after placing a Parts List. 9.True False When creating drawing views from an assembly, you can create views from multiple presentation views or design views. 10.True False A Bill of Materials only retrieves it data from a Parts List.