Inventor Derived Part

Autodesk inventor has a rather practical functionality called the “Derive” functionality. What the Derive functionality does is lets you create a new part to reference an existing part’s solids, surfaces, parameters, work geometry, sketches etc.

The main benefit of this is to be able to create a model that has various parts linked to a base part, then when changes are made to the base part the other linked parts will update as well, this is handy because if you want to make various variations of one part you can also break the link from the derived base part to the derived part. Enabling you to make different parts with different geometry.

A Derive assembly is a new part that references an existing assembly. You add to the new derived part or assembly, when you add new features to the base component or when the base components features are edited, the derived part updates with the changes.

There are two methods in which to create derived parts. The “Push” method and the “Pull” method. We will go through the “Pull” method in some more detail.

One thing to note is that the Derive window that opens, is different depending on whether you

are deriving from a part of from an assembly. This just means that the selection options available and the window layout will be different depending on what you are deriving from.

I’ll go through the window of the Derive Part, showing the most commonly used buttons and then do a part derive example.

Derive Style:

Derive Style Buttons merging

This will create the part as a single solid, removing the seam lines between parts or solid bodies, merging the part and making it look like a single part.

Derive Style Buttons solid merging

This merges the solids into one component but still keeps the edges to make it look like separate components.

Derive Style Buttons multiple merging

This option creates the part with multiple solids.

Derive Style Buttons Work Surface

This is an additional selection to specify whether you want to convert the solids to surfaces.

Status Buttons:

These will visually indicate whether the features in the feature window will be included in the derivation or not.

Status Buttons

Feature Window

The feature window enables you to manually select what you want to add in the derivation or remove, from the original model.

In the picture below, you can select or deselect what you would like to add by clicking the circles to toggle them between green and grey.

The red Arrows are where I have enabled the features, the blue arrow is where I have disabled the feature’s and the green arrows indicating where only some of the feature’s in that category have been enabled and some not.

Derived Part Features

Other Options

Mirror Derived PartThere is also the option to select different design views if they have been created. The scale can also be altered if you require so. You also have the option to Mirror the derived part, and you can then select about which plane you want the part to be mirrored.

Once you are happy with your options click “Ok”.

The derivation will then be created, you will know so by the icon that appears in the browser as such.

Derived Part Example

In the following example I’m going to take you through a typical derivation and what it can achieve.

What we are going to do is create a duct that goes from big too small.

The first step is to create the base geometry, this is going to be the geometry you will have to derive into the other parts that will make up the final Components. You need to think about what you are trying to achieve and create your base geometry to assist you in getting the required result.

I have create a surface model of the ducting to then derive the surface into various sheet metal parts to create the final model that will update and change according to any changes made to the base model.

I’m going to create a user parameter in my base part to define the thickness of the sheet metal used.

Derived Part Parameter

Derived Part Parameter 2

Once you have created all geometry and user parameters, you need to save the base part, then open a new file, in my case I will be using the sheet metal template.

Now activate the derive feature in your new part and browse to your base part. The derive part window will open.

Derived Part Parameter 3

Once the surface model is inside the new part you created, select a side that you want to create the faces on, then create sketches on those faces and project the edges through as follows.

Before you create the solid geometry, in my case I will use the Sheet Metal Face tool, I’m going to set my sheet metal defaults to be equal to the user parameter we derived through.

Sheet Metal Face Tool

Sheet Metal Defaults

I did this to link the user parameter to the thickness of the sheet metal that will be used through the design of these parts.

Sheet Metal

Then Create that face as a solid using the reference geometry as follows

Sheet Metal 2

I’m then going to turn the surface invisible, and save the part as is and then create another 3 parts to get the remaining sides in a solid.

Once all 4 sides where completed I’m going insert all the components into an assembly file. As follows

assembly file

Now one very cool benefit is that if you create your base correctly and you bring all the parts in, you will not need to constrain them together. You must just ground them all at the origin and magic will happen.

ground and root component

All the parts will now jump into place according to your Base model that you started with.

So now for more magic!!!

I’m going to go to my base model and change some geometry. See what happens to my Assembly.

base model

Note the changes on the Base model, save the model with the changes and then go to the assembly. Update the assembly and watch magic happen in front of your eyes.

using derived parts

See the difference, this is the benefit of using Derive parts. The power of this features is very high and depends on your knowledge and setup of the base model.

Hope you found this post useful.