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Back to Basics – 4 Autodesk Inventor Techniques You Should Know

With so much focus given to new features / technologies by CAD bloggers / vendors, it’s easy to forget the little things. I thought I’d start a series of posts that deal with simple, time-saving workflows and tricks that you may have missed along the way while learning to use Inventor.

This first part will demonstrate 4 simple tips / techniques, in a video below:

  1. Two-click Center Workplane
  2. ‘Derive’ Workflow
  3. Convert projected geometry to ‘Construction’
  4. Workplane normal to path for sweep

Two-click Center Workplane

Very often you want to place a workplane exactly halfway between two faces or other planes. By selecting the workplane tool and simply clicking the two faces, you can do just that. In the 2015 release of the product, this workflow was expanded to use any two faces! They no longer have to be parallel, or similar in any way.

‘Derive’ Workflow

I consider this to be one of the most powerful and useful workflows in Inventor. Not only can you use it to maintain adaptive geometry with a source part or assembly, but you can also bring through parameters and work-features, or even use it to mirror or scale a component! Very handy, like these paper towels.

Convert projected geometry to ‘Construction’

I’m sure you’ve all come across that annoying warning: “Cannot constrain or dimension reference or fixed geometry.” This often happens when you think you are clicking on an unconstrained sketch feature, but there’s actually some projected geometry underneath. I find that it helps to project in the geometry you need (within a part only, please don’t use cross-part projection in assemblies!!! Use derive instead) and then turn all of that geometry to construction, before creating your own sketch geometry using the construction features as reference. This will help you to build much more reliable sketches.

Workplane normal to path for sweep

I use this one EVERY time I do a sweep. Often the start of your sweep path is at a point in space with no other reference geometry nearby. This allows you to quickly create a plane on the endpoint that is normal to the path.

Hopefully some of you may find at least one of these tips useful. If you have tips of your own that you’d like to share, please share away in the comments below!

Feature image credit: “Ideal Insurance, Moor Green Lane – 123” by Elliot Brown

Who gives a Flying Function? I do…

Equation Curve in 2D SketchEquation Curve Command in Inventor’s Sketch Environment

The 2D equation curve function has been available in the Inventor sketch environment for a few releases now, but I haven’t seen all that much written about it, and don’t know too many people who are using it. For those reasons, I thought I’d do a quick post with an example of it’s use.


Before it effectively became NASA in 1958, NACA (National Advisory Commitee for Aeonautics) was a U.S. Federal Agency that was set up to undertake, promote and institutionalize aeronautical research. One of the important results of their research was the development of a series of aerofoil profiles, in the 1940s, that are still in use in aircraft and marine design today. A NACA aerofoil is one whose shape is determined by one of a series of mathematical equations. In this example, I used the “4-digit” symmetrical equation to create a non-cambered aerofoil. My next challenge is to create a cambered profile using the relevant equation.

The Math

The following is an excerpt from this wikipedia entry:

Equation for a symmetrical 4-digit NACA airfoil

Plot of a NACA 0015 foil, generated from formula

The formula for the shape of a NACA 00xx foil, with “xx” being replaced by the percentage of thickness to chord, is:[3]

 y_t = \frac{t}{0.2}c\, \left[ 0.2969 \sqrt{\frac{x}{c}} + (-0.1260) \left(\frac{x}{c}\right) + (-0.3516) \left(\frac{x}{c}\right)^2 + 0.2843 \left(\frac{x}{c}\right)^3 + (-0.1015) \left( \frac{x}{c} \right)^4 \right],[4][5]


  • c is the chord length,
  • x is the position along the chord from 0 to c,
  • y is the half thickness at a given value of x (centerline to surface), and
  • t is the maximum thickness as a fraction of the chord (so 100 t gives the last two digits in the NACA 4-digit denomination).

The Model

I created a 2D sketch in Inventor 2015, and used the equation curve tool (hidden in the “Line” dropdown menu) to input the formula above.

Inventor 2D Equation Curve2D Equation Curve in Inventor Sketch Environment

If you’d like to recreate this, here is the formula in a copy-paste-able format:

( ( t / 0.2 ul ) * chord ) * ( ( const1 * sqrt(x / chord) ) – ( const2 * ( x / chord ) ) – ( const3 * ( ( x / chord ) ^ 2 ul ) ) + ( const4 * ( ( x / chord ) ^ 3 ul ) ) – ( const5 * ( ( x / chord ) ^ 4 ul ) ) )

The equation only creates one half of the curve, so I used the mirror tool with the “Self Symmetric” option ticked to get the leading edge. The trailing edge is a very short vertical line.

The iLogic (of course there is iLogic, it’s me, iGav)

It’s all well and good to have a static aerofoil section for an example, but for any practical application, you’d want to be able to adjust the shape and parameters to get exactly the shape you require. An iLogic form provides a really easy-to-use interface for adjusting the chord length and thickness of the section.

A form to adjust the aerofoil modelAerofoil Parameters can be Adjusted with an iLogic Form

While I was there, I thought I’d add a wing plan sketch with some control planes and a series of stations. This turns the aerofoil section into a wing shape and allows me to adjust the leadin and trailing edge taper angles.

If you’re interested, here’s the Inventor 2015 model file: Aerofoil iLogic Model

 If any of you have a particular equation for something interesting, that you’d like to see applied to a model, please get in touch.

Feature image credit: simpleinsomnia – “Students study an equation on a chalk board” – Unedited


Time to Tame the Beast! Learn to Customize Autodesk Inventor

Autodesk Inventor API - Object Model

Recently, a friend (and colleague) asked me how I go about planning the development of a new application or customisation project. He already has a pretty good handle on code structure and syntax, but struggles to know where to start in actually bringing his idea to life. In his words, he suffers from “the worst kind of writers’ block.” I totally sympathise with this issue as I have the same problem myself, quite frequently. The truth is, unless I’m working on a commercial project that has been carefully scoped, budgeted and scheduled, most of the time I just ‘hack’ something together. Having said that, there are definitely a couple of tips and tricks I can share which should help novice coders get started with customising Autodesk Inventor. If there is enough interest, I could do a similar article on the Vault equivalent.

I’m going to split this up into a couple of categories:

  1. Interrogating a live document to learn from and capture information
  2. Writing pseudo code to figure out the ‘flow’ of your program

Interrogating a live document

Usually when I start working on a customisation job, I only have a rough idea of what I want to achieve. With a limited mental picture of how the finished tool may look, often the only thing I know at the start, is the rough area of Inventor I’ll be working with. For example, if I’m building a tool to ensure that the designer fills out all the appropriate metadata for a model, I know straight away, that I’ll be working a lot with iProperties.

Autodesk Inventor API Documentation

API Documentation for Autodesk Inventor

To find out more where these objects are stored, and how they interact with other objects, you need a reference. The API documentation for Inventor, while thorough, is pretty dry to read and can be difficult to navigate if you’re unfamiliar with it. By using the little trick below however, you can see the API objects in a live document, populated with real data, which makes it a lot easier to understand. Let’s say, for example, you’re looking for the “Work Point” object that represents the origin of a particular part. Now of course can go into the model browser and find it, but what if you want to access it programmatically, where does it live in the structure of the model document? Watch the video below to see how to get this information quickly.

Interrogating the Open Document in Inventor VBA Environment

The API is a complex beast, with a lot of objects, and a deep structure. To give you a head-start, the table below lists a few of the objects and collections that I use most often.

Object / Collection Contains
Document.ComponentDefinition Parameters / Constraints / Work Geometry / Occurrences / Mass Properties
Application.Documents File Operations (Open, Save etc.)
Document.Materials Materials
 Document.PropertySets iProperties
 Document.ReferencedDocuments Document References


Before diving in to the actual code, I find it is often helpful to design the logic and flow of the program by using diagrams like flowcharts. Additionally, writing out the decisions that need to be made, in plain English, can help get things clear in your head. Writing pseudo code allows you to get the structure down quickly, without worrying about the syntax and intricacies of the programming language that you will be working in later. So what is pseudo-code exactly, you may ask? I’ll try to explain with an example.

Let’s say that we have a model of a box, whose length can be manipulated. Additionally, it’s colour is dependant on it’s length. Short boxes are red, medium ones are yellow, and long ones are green.

  • Maths
    • Length < 150mm — Red
    • 150mm <= Length < 250mm — Yellow
    • Length >= 250mm — Green
  • Plain English – If the length of the box is less than 150mm, then make it a red colour. If it’s length is between 150mm and 250mm, then make it yellow, and if it is longer than 250mm, then make it green.
  • Pseudo-code



  • Actual code ( for example)

VB Code

Hopefully these techniques give you some confidence to get stuck in and try your first Inventor customisation project. While I’d suggest you begin with iLogic rules and forms, sometimes you hit a wall with iLogic’s scope, and you need to delve into the API to access the areas you want to work with.

’til next time…

Design & Motion are Between The Lines

Keeping Up Appearances with Autodesk InventorJust a quick post to let our readers know we have a Guest Post on Shaan Hurley’s legendary Autodesk Blog Between The Lines. Given the historical significance of Between The Lines with respect to CAD blogging, I’m pretty stoked to have finally got some work up there. Keeping Up Appearances with Autodesk Inventor shows Inventor power users how to ‘window select’ multiple faces, so they can apply appearance overrides in one hit. So please go take a look and hopefully you lot can put it to good use.

iLogic Assemblies – It’s wise to normalise!

Here’s a quick tip for those who have discovered the power of iLogic in Inventor.

When creating configurable Inventor assemblies using iLogic, there’s a process that you should follow when it comes to naming your components. It’s called “normalising” (or “normalizing for you Americans), and it will make dealing with multiple unique instances of your assembly a lot easier.


As promised in the video, I have attached a copy of the dataset for anyone who is interested in seeing how it was constructed or to take a look at the code. Here it is:

iLogicBox Model

(Feature image mashup, credits: Ruth Hartnup – “All her eyes are evil”  and Monica Arellano-Ongpin - “Los ojos de un hombre”)


Autodesk Inventor 3D Sketch Bends Ease Tube Transitions

I prefer to work in the 2D environment when possible. It’s easier to control factors, but there are times when the 3D sketch environment saves a lot of time, and times where a 3D sketch is simply the only option.

3D Tube Bend Render in Autodesk Inventor

One such instance is routing tubing from a non-orthogonal axis fitting to a mount on an orthogonal axis. I could have used multiple 2D sketches to develop multiple work features in order to handle the transition, but what a waste of time. Plus with those extra steps, the design history gets quite complicated and begging for update failures.

3D Bend

Using a 3D sketch to layout linear geometry and 3D Bend to control the bend transitions is quite easy.  In my example, I have both mounting axes, as well as 2D geometry which delineates start and end segment tube definitions. All I need is the stuff in between.

Autodesk Inventor 3D Sketch Geometry with Work axes

  • Create a 3D sketch, and ‘Include’ all the 2D geometry that is needed as a reference.
  • Draw Line geometry representing the linear segments that are needed in the transitions.
  • Constrain the lines as needed to the references.
  • Add Dimensional constraints as needed.
  • Create 3D Bend at each vertex.


Autodesk Inventor 3D Sketch Bend Geometry

Some Tips

In order for 3D Bend to work, all related linear geometry must be in the same 3D sketch. It will not work on geometry in more than one 3D sketch.

When you use the ‘Include Geometry’ tool, any geometries included can be used in a Sweep operation. In the video below, I demonstrate how included geometry can be used as part of the path in a Sweep. Note that if you want that included geometry to be ignored, just like in 2D sketches, you have to change their type to construction.

A path driven sweep will fail if your included geometry (non-construction) overlaps your sketched geometry. Essentially doubling back on itself. This will cause the Sweep to fail. Since the problem is covered up by well built line-work, it is often very difficult to discover this.

How Does It Update?

Brilliantly! I started with the tube ending all the way up to the flange, but realized that I needed room for a tube hinge  I simply adjusted the 2D sketch references for the gap needed and the updates behaved perfectly.

Autodesk Inventor 3D Sketch Tube Surface Transition

Video Demo on our YouTube Channel