Introduction: TAD 330- Making Isometric & Exploded Assembly View Drawings

The following will show you how to create the first two pages of the engineering design packet for TAD 330, which are the isometric & exploded views of a completed assembly.


  • Completed .iam assembly file created in Autodesk Inventor (the 2019 version is used here)

Step 1: In Inventor, Create a New Drawing (.idw).

  • Open Inventor.
  • Select File->New->Drawing
  • Click ANSI (mm).idw

Step 2: Format the Drawing Size

  • Under the "Drawing Resources" tab,
    • Select "Sheet Formats"
      • Select "B Size, 2 view"

Step 3: Import Your Assembly File Into the Drawing

  • After selecting B size, a prompt will appear to select the document you wish to include in the drawing.
    • Select the document.
    • Click "Open", then click "OK".

Step 4: Open the Drawing and Delete View 1

  • Delete the view that Inventor automatically applies, since an isometric view of the assembly is needed.

Step 5: Under "place Views", Create a New Base View

Step 6: Format the New Base View

  • The view will need to be adjusted so that it is isometric.
    • Click the "Home" icon on the navigation cube to orient it correctly.
  • The scale used in this example is 1/2
  • The correct style for all isometric projections is shaded with no hidden lines visible.
  • Click "OK" once all of the above steps have been completed.

Step 7: Center the Isometric Base View

  • Center the isometric projection of the assembly to make it look presentable.
  • Remember, this is the very first page of the design packet!

Step 8: Create a Text Box & Fill Out Title Block Info

  • Under the "Annotate" tab, click on "Text"
    • This will allow you to create a text box anywhere on the drawing.
  • In the box above the "TITLE" block, make a text box and type "BEREA COLLEGE" in 9.53mm font.
  • In the larger title box below, make a text box and put the name of the assembly in 7mm font.
    • In this example, it is the Leveling Assembly from Chapter 12.

Step 9: Create a New Sheet for Page 2-- the Exploded Assembly View

  • Under "Place Views", click "New Sheet".

Step 10: In Order to Create an Exploded View of the Assembly, Create a Presentation

  • "File"-->"New"-->Presentation--> Standard (mm).ipn
  • Click "Create".

Step 11: In the Presentation, Select the Assembly File.

  • Once the assembly file has been selected, click "Open".

Step 12: Explode the Assembly

  • To explode the assembly, click "Tweak Components".

Step 13: Select and Explode Multiple Parts

  • While holding down the "Ctrl" key, select the parts which you would like to move together.

Step 14: Tweak the Lifting Block Up 180 Mm

  • Ensure that both "Tweak Components" and the Lifting Block part are selected.
  • Click on the direction arrow pointing upwards (Y-axis).
  • In the dialog box, type in "180".
  • The part will then move upwards by 180mm.
  • Click the green check to confirm this movement.

Step 15: Tweak the Sliding Block and Adjusting Screw Up 120 Mm

  • Ensure "Tweak Components" is selected.
  • Use Ctrl + click to select both the Sliding Block and Adjusting Screw.
  • Click on the direction arrow pointing upwards (Y-axis).
  • In the dialog box, type in "120".
  • The parts will then move upwards by 120mm.
  • Click the green check to confirm this movement.

Step 16: Tweak the Adjusting Screw 100 Mm to the Right

  • Ensure "Tweak Components" is selected.
  • Select the Adjusting Screw.
  • Click on the direction arrow pointing to the right (Z-axis).
  • In the dialog box, type in "100".
  • The part will then move 100mm to the right.
  • Click the green check to confirm this movement.

Step 17: Be Sure That the View of Individual Parts Is Unobstructed.

Step 18: Take a Snapshot View of the Fully Tweaked Assembly.

  • Under "Presentation", click "New Snapshot View".
  • This will take a snapshot of the tweaked assembly, so it can be used in a drawing.

Step 19: Save the Presentation File.

Step 20: Import the Snapshot View to the Drawing.

  • On Sheet 2 under "Place Views", click "Base"
  • The exploded assembly should automatically pop up.
    • If it does not, search for the right file before continuing.

Step 21: Format the Exploded View.

  • Be sure to format and orient this exploded view in the same way as the non-exploded isometric view on page 1.
    • No hidden lines, shaded, and same scale (in this example, 1/2).
  • Offset this view to the left side a bit as room will be needed to fit the parts list and balloons.
  • Click "OK".

Step 22: Create a Parts List.

  • Under "Annotate", select "PartsList".
  • Select the exploded view as the document you wish to have a Parts List for.
  • Click "OK".
  • An outline of the Parts List box will appear; drag this to the top right corner of the drawing.

Step 23: Edit the Parts List to Include "Material" Column Instead of "Description"

  • To execute this, double-click on the Parts List.
  • A dialog box will pop up.
  • In this box, select "ColumnChooser" (the leftmost button).
  • In the "Selected Properties" column, click on "Description", then select "Remove".
  • Under "Available Properties", click on "Material", then select "Add" to add it to the "Selected Properties" list.
  • Click "OK".

Step 24: Neaten the Parts List

  • Get rid of unnecessary spaces in the parts list by dragging the columns left or right to minimize them.

Step 25: Under "Annotate", Select "Auto Balloon".

  • Balloons will allow the parts in the exploded assembly to be easily identified and compared against the parts list.

Step 26: Click All Parts in the Assembly to Automatically Bring Up the Balloons

  • To make sure all of the parts in the assembly have a balloon, ensure that when a part is selected, it turns blue.
  • All the blue-outlined parts will have a balloon designated to them.

Step 27: Right Click, Then Click Continue

Step 28: Drag the Balloons Away From the Exploded View, Then Click to Place Them.

  • After placing the balloons, click "OK".

Step 29: Neaten the Balloons

  • For maximum neatness, ensure that the balloons are somewhat aligned to each other, or that their lines are parallel.

Step 30: Place Title Block Information.

  • Instead of creating new text boxes for sheet 2 and typing the same information, the text boxes created in sheet 1 can be copied and pasted into the title block in sheet 2.
  • When pasting the copied boxes into sheet 2, the outline of two boxes will appear in green.
  • Align them within the title blocks and then left-click to paste.
  • Press the "Esc" key once complete.

Step 31: Page 1 Isometric Assembly View and Page 2 Exploded Isometric Assembly View Complete

  • The first two pages of the engineering design packet are now complete.