· Creating a Part

· Adjusting program settings

· Sketching and dimensioning

· Navigating in sketch mode

· Sharing sketches

· Revolving and extruding sketches

· Adding chamfer and hole features

· Quick Start

· Organize files into projects

· Assigning a Project

· Close all files

· File > Projects

· Select tutorial files

· Done

· Now tutorial files can be accessed (page 3)

· Start a new part file

· Sketch mode gets enabled

· File > New

· Click Metric Tab

· Double click Standard (mm).ipt

· Origin is at center of window

· 2D Sketch Panel is present with sketch tools (page 5)

· Things to know about tools

· Related tools accessed by clicking arrow if present

· Tooltips present

· Icons for tools not available in present environment are dimmed (page 6)

· Adjusting sketch grid settings

· Tools > Document Settings > click Sketch Tab

· Use following settings:

· X/Y snap spacing: 1 mm

· Snaps per minor line: 2

· Major line every 5 minor lines

· Click OK (page 7)

· Adjusting Sketch Grid Display

· Tools > Application Options > Sketch Tab

· Display grid, axes, and minor lines

· Make sure Snap to Grid is selected

· Click OK (page 8)

· Building Parts

· Nozzle for valve assembly (page 9)

· Overview: Builing a Part

· Create a base sketch

· Add dimensions to constrain sketch

· Revolve sketch about axis (page 10)

· Overview: Adding Features

· Share sketch so we can add geometry

· Add constraints and dimensions

· Use new geometry to add two new features (page 11)

· Create First Sketch

· Start at origin

· Three line segments

· Vertical 27 mm

· Horizontal (-ve x) 24 mm

· Verrical (-ve y) 6 mm

· Right click and Done (page 14)

· Two more line segments

· From origin (-ve x) 10 mm

· Close the loop with end to end line (page 15)

· Save part as my_nozzle.ipt

· Allow save to exit sketch mode (page 16)

· Part Features Panel replaces Sketch features panel

· Click Sketch Tools in Inventor Standard toolbar

· Click top horizontal line in sketch

· Back in sketch mode with 2d sketch panel

· Ready to add dimensions (page 17)

· Dimension sketch

· Click General Dimension tool

· Dimensioning Notes

· Precise input as we dimension

· Right click graphics window

· Select Edit Dimension

· Double click dimension if Dimension tool is inactive

· Specify font and scale for sketch dimensions

· Tools > Application Options > General Tab

· Enter an annotation scale value

· Select a font from Text Appearance list (end dimensioning notes) (page 18)

· Save often

· Display tools

· Add Zoom Selected to other obvious tools

· Pan with Wheel button down (page 19)

· Create First Feature

· Rotate to view x-y plane vertical

· Click Revolve tool

· Click right vertical line for axis (page 20)

· Complete the feature

· Click OK

· Click Save tool (page 21)

· Controlling Part Color

· Select from color list in Standard toolbar (page 22)

· Share First Sketch

· Expand Revolution1 in browser

· Right click Sketch1 and select Share Sketch

· Sketch becomes visible on part (page 23)

· Return to sketch mode to add geometry for next feature

· In browser right click Sketch1 and select Edit (page 24)

· Return to planar view

· Click Look At tool and the top horizontal line or any other line to return to planar view of sketch (page 25)

· Add Geometry to Sketch

· Use grid snaps and drag with line tool to draw arcs (page 26)

· Click Line tool

· Start at 6 mm to left of origin

· Draw vertical line down 10 mm (page 27)

· Create the New Loop

· Click and hold mouse down

· Drag to right to draw arc of radius 6mm

· Draw vertical line up

· Close loop by returning to start point (page 28)

· Constrain Sketch

· Add two dimensions to constrain

· Add one more dimension to position relative to existing sketch (page 29)

· Update and Save Work

· Click Update tool on Standard toolbar

· Rotate to view similar to isometric view with large face on top (page 30)

· Create Extruded Features

· Because it is shared the sketch can be used to create a midplane extrusion

· Use same sketch to cut material from extruded feature (page 31)

· Create First Extrusion

· Click Extrude tool

· Select area in second sketch

· Use Midplane and 12 mm Distance

· Click OK (page 32)

· Create Second Extrusion

· Click Extrude tool

· Select same loop

· Distance = 6 mm

· Click Cut button

· Click Midplane button (page 33)

· Click OK to create extrusion

· Save

· Ready to add last two features to nozzle (page 34)

· Create Chamfered Edge

· Click Chamfer tool

· Click top edge of part

· Distance = 2 mm

· Click OK to accept preview (did not see preview) (page 35)

· Add a Hole

· Through two tabs just created

· Click Hole tool

· Placement: Concentric

· Plane reference: Pick front tab surface

· Concentric reference: Select circular edge of tab (page 36)

· Diameter: 6 mm

· Termination: Through All

· Click OK (page 37)

· Summary

· Set up environment

· Create simple sketch

· Add and edit dimensions

· Create extruded features

· Share sketches

· Add geometry to existing sketches

· Create chamfer features

· Create hole features

Resume

Inventor Skills

Creating Adaptive Parts in an Assembly

Using Frame Generator

Creating iFeatures

Using Content Center

Creating a Part

Building Sheet Metal Parts

Creating Assemblies

Creating a Bolted Connection