Autodesk Inventor modelling – Pattern a feature around a coiled path

Shafts and gears are common components in many engineering designs. We are often required to design shafts for mechanical machines that do heavy rotational work, such as those in mines or food processing industries. This, more often than not, requires features or components to be patterned along the length of the shaft. It may not be too much trouble to do if the pattern was linearly along the shaft, but how can we pattern, for example, spokes along a curved coil path with its axis along the shaft center? (See featured image).

Here is a quick guide on how that can be achieved.

Step 1

Draw your shaft and plan your length and diameter accordingly. You may need to reference these dimensions later.

Step 2

Create an offset plane using an axis from any plane passing through the center of your shaft, in this case, I used the XZ origin plane.


Step 3

Draw the feature or body which you wish to repeat. In this example, I am drawing a simple rod with threads at the top end. Your extrusion does not need to match my settings and parameters, and the feature you design is really up to you. As long as you are able to pattern it and the associated features, there won’t be any issues going forward.

Step 4

Now, start a 3D sketch and use the helical curve tool to draw a coil along the length of the shaft. In this case I used pitch and height to drive my coil, but depending on your design requirements, you may use, pitch and revolution or any other criteria from the drop down menu.

Match the diameter to that of your shaft and account for any offset which your initial feature may have. In this case, I made the curve height shorter than the total shaft length of 1520mm as the bolt extrusion I drew was offset by 20mm.

Pay careful attention to the data you have input in this curve as this governs the way the features will pattern. For example, if you are designing around a linear distance between features, you would need to use some mathematics to determine the coil pitch as this is defined as the distance of one complete revolution.

Step 5

Now that we have a path to follow, use the rectangular pattern tool in your ribbon. Yes, that may sound counter-intuitive, but it is indeed the solution.

Once you’ve entered the rectangular pattern dialogue box, follow the settings shown below:

Select the feature or component you wish to pattern. Here I have selected my threaded rod.

Enter the number of features you want, again, if you’re working with a linear pitch between objects, some simple maths is required as this is the total number of features to be patterned.

There is only ONE direction and it is the helical curve that needs to be selected. Set the direction type to curve length and then press the expand dialogue box button for advanced settings. (>>)

In the compute tab, keep setting as identical, in the orientation tab, use Direction 1 (which we set to the helical curve sketch).

This will give you a preview as shown above.


That’s it, you’re done. You should have successfully patterned your feature around a helical curve as seen below. That wasn’t too difficult, was it?


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