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Creating Drawings in Inventor

This workshop will teach now to create professional technical drawings. We will go over base and projected views, how to fully dimension a part and section a part. To read more about engineering drawings, see: Engineering Drawings

For this tutorial, download the part: bracketDrawing.ipt


Part 1: Creating a drawing file

Download and open bracketDrawing.ipt from the website.

Create a new .idw file. and click the leftmost button “Base”. If you do not have bracketDrawing.ipt open you will have to browse for the right file. Change the scale to 5:1.

Click ok or click on the place where you want the part to be.

This automatically starts the “Projected” tool which allows you to place different 2D and 3D views of the part. Click to create a top and right view. When finished, right click and choose create.

Double click on the top right view and select shaded to make it a solid looking part. To move individual views around on the page, click them once to select them, then click and drag the red dotted box surrounding them.

Part 2: Dimensioning Parts

When dimensioning a part, you want it to be “fully dimensioned”. This means you give enough information so that every feature is defined without being redundant.

Go to the Annotate tool bar and select general dimension at the top left.

Click the following lines just like you would when you dimension sketches.

Continue dimensioning until you have done the following:

In drawings, it is useful to include center marks for holes. Use the following command and click both the inner circle and outer top curve:

Now use the “Chamfer” tool to mark the chamfer. Click 2 of the hidden lines to create a chamfer note. The first line you click is the noted one and the second is the reference one.

This view is now has all the dimensions it needs.

Part 3: Dimensioning the Remaining Views

This view has 2 flanges that stick up and are the same thickness. Dimension the thickness of one of these flanges and then click again on the number to bring up the following window:

The symbol “<<>>” is the numeric value that is being dimensioned. Type “X2” after the “<<>>” to show that there are 2 flanges of the same thickness.

Add the other 2 dimensions shown below:


Note: We don’t give the dimension of the total height because we already gave that in the last view. Don’t repeat dimensions between views.

We will now dimension the top view. Select the “Hole and Thread” tool from the Annotate menu.

Now click the dotted line in the top view to give the bolt information. This information is available since we used the “hole” tool when modeling the part.

Center mark the hole. 

Part 4: Editing Drawing Information

We will now change the information in the bottom right of the drawing. This is used to keep track of approval and who has seen or edited the part. To edit this information, click the Inventor icon at the very top right and select iProperties.

Here you can edit the information that will appear in the lower box. Be sure to type in ALL CAPS since that is the engineering standard.

Daniel Yang,
Oct 20, 2015, 12:39 PM