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Unit 06 · Lecture 11

Drawings: base, isometric and section view

A drawing is how a part reaches the workshop. This lesson sets up an A4 DIN sheet for the curved disk and places its three views: front, isometric and section A-A.

Video 14:58Reading 9 minUpdated 26 October 2026

Lecture video, 14:58. The written steps below follow the video, with timestamps for each part.

What you will build

An A4 landscape drawing of the curved disk with a filled-in title block, a 1:1 unshaded front view, a 1:2 shaded isometric view and a hatched section A-A.

You will learn

  • DIN.idw vs. DIN.dwg
  • Edit Sheet: size and orientation
  • What the title block and revision table record
  • Drawing scale is for display, not manufacture
  • Base, projected and section views

Before you start

You need the curved disk part file saved. A drawing reads from the part.

Step by step

  1. 01

    Choose IDW or DWG

    0:42

    In File → New → Metric there are two DIN drawing templates (enlarge the dialog if one is hidden). DIN.dwg opens in many CAD programs. DIN.idw is Inventor’s own drawing format. Use IDW.

  2. 02

    Set the sheet to A4

    2:13

    Right-click the sheet in the browser and choose Edit Sheet. Change the size from A2 to A4 and keep it landscape. The title block seems to grow, but in fact the sheet shrank around it.

  3. 03

    Fill in the title block

    3:36

    The title block sits bottom right and its position follows the projection standard. It records revision (0 for a first issue), date, drawn and checked by, standard, projection symbol, material and units. The file name fills in itself when you save as Curved Disk.

  4. 04

    Place the base view

    7:16

    Place Views → Base View, choose Curved Disk, front orientation. Set the scale to 1:1, style unshaded, and turn on Toggle Label Visibility so the view name and scale show.

  5. 05

    Remember what scale means

    7:57

    A 1:2 scale doesn’t mean doubling dimensions. Dimensions are always true size. Scale only shrinks or enlarges the picture so it fits the sheet.

  6. 06

    Project the isometric view

    10:05

    Use Projected View from the base view, or just drag diagonally from it. Moving straight down, up or sideways gives orthographic views. With Inventor’s default first-angle projection, the top view lands below and the left view on the right. Drag to the bottom-left corner, right-click → Create, then set it to shaded, 1:2, named Isometric.

  7. 07

    Create section A-A

    12:53

    The third view on the reference drawing has hatching and an A-A label, so it’s a section, not a side view. Choose Section, pick the base view, snap to the centre line, click above and below the part, then right-click → Continue, and place the section beside it.

Drawing standards

First- vs. third-angle projection

Europe (DIN/ISO) uses first-angle projection: a view appears on the opposite side of the object it is seen from. North America uses third-angle, where views appear on the same side. The title block symbol says which one applies, so always check it.

Section views

A section cuts the part along a line such as A-A and shows the cut faces hatched. It reveals internal features such as holes, pockets and wall thickness that an outside view would hide.

Common mistakes

Practice exercise

Add a second sheet to the same file and place the curve part at 1:1 with a section through one threaded hole.

Check yourself

Which drawing format is Inventor’s own?

.idw.

A view is at 1:2. Do you double its dimensions?

No. Scale affects only the picture.

In first-angle projection, where does the top view go?

Below the front view.

What tells you a view is a section?

The cutting line with labels such as A-A, and hatched faces.

Want the graded version? Take the 5-question lesson quiz in the course player after the video.

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.