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Unit 01 · Lecture 1

Introduction to Inventor 2027: your first part

This first lesson takes you from an empty Inventor window to a finished 3D part: a simple cylinder. On the way you learn the decisions every new part starts with: which template, which file type and which plane to sketch on.

Video 10:37Reading 7 minLevel: beginnerUpdated 26 October 2026

Lecture video, 10:37. The written steps below follow the video, with timestamps so you can jump to each part.

What you will build

A Ø75 × 100 mm cylinder, roughly the body of a bottle. You will start it at Ø50, then change the sketch and watch the 3D model update itself.

You will learn

  • Choosing the metric Standard (DIN).ipt template
  • Editable (IPT) vs. non-editable (STEP, PDF) files
  • Origin planes, the ViewCube and the coordinate triad
  • Sketch → Extrude → edit in the model browser

Before you start

Install Autodesk Inventor Professional 2027. Students and educators can get a free educational licence from Autodesk; everyone else can use the 30-day trial, which is enough to complete this course.

Step by step

  1. 01

    Create a new part from the metric template

    0:46

    Go to File → New. If the dialog opens in the en-US folder, the templates there use inches. Switch to the Metric folder and choose Standard (DIN).ipt.

    DIN stands for Deutsches Institut für Normung, the German standards body. Its standards are used widely across Europe. The template sets millimetres as the unit, and every dimension in this course is in millimetres.

  2. 02

    Pick a standard part, not sheet metal

    2:06

    The part templates come in two kinds. A standard part is a solid body built from profiles with depth. A sheet metal part is made from a sheet of constant thickness that you bend and fold (that comes in Unit 04). Choose the standard part and click Create.

  3. 03

    Start a 2D sketch and choose the plane

    4:15

    Every 3D feature starts from a 2D sketch. Click Start 2D Sketch. Three origin planes appear at the centre of the screen: XY, YZ and XZ. You will also find them, with the X, Y and Z axes and the centre point, in the Origin folder of the model browser on the left.

    Think about how the finished part will sit. A bottle stands on a table, so seen from above it is a circle. Use the ViewCube (top right) to go to the Top view, then check the coordinate triad (bottom left). The plane facing you in Top view is XY. In Front view it is XZ, and in Right view it is YZ. Select the XY plane.

  4. 04

    Draw the circle

    7:00

    Choose Circle, click the sketch origin as the centre, drag outwards and type 50 for the diameter. Press Enter. You now have a closed profile, a shape the software can turn into a solid.

  5. 05

    Extrude the profile into a cylinder

    7:44

    Click Finish Sketch to return to the 3D Model tab, then choose Extrude. Extrude adds depth to a profile. Select the circle as the profile. The extrusion starts from the sketch plane (XY).

    Look at the direction options: Default extrudes one way, Flipped extrudes the other way, Symmetric splits the distance equally on both sides, and Asymmetric lets you set two different distances. Keep Default, enter 100 mm and click OK.

  6. 06

    Edit the sketch from the model browser

    9:07

    The model browser is your part’s timeline. Expand Extrusion1 to find Sketch1 inside it. Double-click Sketch1, change the diameter from 50 to 75 and click Finish Sketch.

    The cylinder grows straight away. The sketch drives the feature, so you change the shape by changing the sketch, not by rebuilding the solid. This is the core idea of parametric modelling.

Key ideas

Editable vs. non-editable files

An .ipt (Inventor part) file keeps every sketch and feature, so anyone who opens it can change the design. In industry you usually keep native files in-house to protect your design data.

To share a part for review or reference without exposing its history, export it as a STEP file. A STEP file is like a PDF of a Word document: the geometry is all there, but the feature history is gone.

Parts and assemblies

Each physical component gets its own part file. A real bottle (body, cap, label) is several parts put together in an assembly, which you will build in Unit 05.

Common mistakes

Practice exercise

Make a new part and model a coin: a Ø25 mm circle on the XY plane, extruded 2 mm with the Symmetric option. Then edit the sketch to Ø23.25 mm (the size of a euro coin) and confirm the solid updates.

Bonus: draw the same cylinder on the XZ plane and compare how it sits in the Home view.

Check yourself

Which template gives you millimetre units in this course?

Standard (DIN).ipt, from the Metric folder.

You want a supplier to see your part but not edit its features. What do you send?

A STEP file. It carries the geometry without the editable feature history.

Which origin plane faces you in the Top view?

The XY plane.

How do you make an extruded cylinder wider without redrawing it?

Expand the extrusion in the model browser, double-click its sketch and change the circle’s diameter.

Written by the CADsmit instructor from the lecture recording and checked in Autodesk Inventor Professional 2027. Last updated 26 October 2026. Spotted an error? Tell us.