The CAD Setter Out’s Autodesk Inventor iFeatures Primer

Autodesk Inventor’s iFeatures are a handy time saving tool, that allow you to save a feature (or a set of features – even a whole part) out to a separate file so that you can re-use it later.

An example of an Autodesk Inventor iFeature that has been placed

iFeatures can be fully Parametric with both size and position driven by Parameters. Like all Inventor features, they are History based and will require some existing features to be placed on ( this could be a work plane, it doesn’t have to be a solid unless the iFeature is a ‘Cut’ extrusion). The iFeature may contain a help file to demonstrate how it should be placed.

Placing an iFeature will always follow the following process:

  • Select – Select the iFeature you want to use
  • Position – Place the iFeature according to the instructions
  • Size – Change the size of the iFeature, or accept the defaults. iFeatures can also have additional custom parameters, which can be changed during the insertion process. These iFeatures are ‘Exposed’ with in your part, so that you can link them in with your existing parameters.
  • Precise position – Many iFeatures allow you access to the original sketch, which allows you to tie the iFeature in with the rest of your models geometry.


To Insert an iFeature

To insert an iFeature from Inventors built in Catalog:

Ribbon: Manage tab > Insert panel > Insert iFeatureInsert an Autodesk Inventor iFeature


This will open the browser at Inventor’s iFeature catalog.  Select any file that has an .IDE file extension.

Or click on the Drop down below to pick directly from the iFeature Catalog.

Insert an iFeature directly from the drop down panel on Autodesk Inventor's Ribbon


In this example I’m going to pick the ‘Semi_sphere’ iFeature from the gallery drop down.

Inserting an iFeature from Autodesk Inventor's standard Catalog


You will see the ‘Insert iFeature’ dialog box . In this case you can see that you are being prompted to pick a plane. Hovering over the plane shows a preview of what you might get.

Positioning an Autodesk Inventor iFeature

Once you have selected the placement inputs ( in this case – the face of the existing feature), you will be given the option of changing the ‘Normal’ direction of the feature (which side of the base plane it’s pointing), aligning it to an existing feature, or rotating it. When you’re done click ‘Next >’.

Tip: If you want to accept the defaults, you can click ‘Next >’ straight away – or just skip straight on to ‘Finish’.

Re-sizing an Autodesk Inventor iFeature during placement

Tip: Note here that the ‘i’ button is greyed-out – so there is no placement help for us to refer to with this iFeature file.

Moving the placement position of the iFeature graphically

You can change the position of the iFeature on the screen – as well as in the dialogue.

Moving an Autodesk Inventor iFeature during placement

To move the feature, click on the crossed lines at the centre of the on screen preview.



Rotating an Autodesk Inventor iFeature during placementTo rotate the iFeature, click on the Arc at the center of the on screen preview.



In both cases, once you have the iFeature where you want it, click on the screen again to finish the Move/Rotate and move the focus back to the dialogue.



Hitting ‘Next >’ Gives us the option to change the value of any of the custom parameters that have been built into the iFeature. In this case the only custom parameter is ‘Radius’.

Changing the parameter values of an iFeature during placement

Precise Position

The final page of the dialog box asks us what we would like to do next. In this case I’m going to chose ‘Activate Sketch Immediately’ so that I can precisely place my part in relation to the rest of my model.

Activating an iFeature's sketch on placement

Here I’ve projected the corner points through, and added a construction line. I’ve constrained my iFeature to the mid point of the construction line so that my iFeature will always be centred.

Adding construction geometry to place an Autodesk Inventor iFeature

Upon closing out the sketch – the feature is placed:

The Autodesk Inventor iFeature is placed

Editing the iFeature

There are two options for editing the iFeature once it has been placed, Parametrically or using the Edit iFeature command.

By opening the Parameters manager, I can see one new parameter that has been added. If I want to change my feature later on – I can change it here. I could also link it to the overall size of the Part from this dialog.

The iFeatures parameters are available from the Inventor parameters manager.

The iFeature shows up in the Parts Feature Tree. You can edit the iFeature at any time by right clicking on it and choosing ‘Edit iFeature’.

Editing an Autodesk Inventor iFeature

There are many iFeatures in the standard Autodesk Inventor Catalog – Why not try a few out today!

Testing iFeatures from the Autodesk Inventor Catalog


To find out how to download and use free iFeatures from the Internet read – What every Drafter needs to know about Autodesk Inventor’s iFeatures.

One Response to “The CAD Setter Out’s Autodesk Inventor iFeatures Primer

  • Ben Gee
    7 years ago

    I’ve been using Inventor for years, but never really used I features! Might give it a go tomorrow