Design of Movable Parts and Assembly


  1. Design of a movable hinged joint
  2. Introduction to Fusion 360 assembly and fitment
  3. Kinematic analysis to check design feasibility


For this project, you will need

  1. Autodesk Fusion 360 on your computer

Let’s begin!

In the previous unit, we learned how to design a static case for the raspberry pi. In Fusion360, one of the biggest advantages is that we can also design and perform the kinematic analysis of movable parts. We will take a look at a simple hinged joint which finds applications in several robotics applications. Follow these steps to get started with the fabrication of a hinged joint, which can later be 3D printed.

  1. Open Fusion360 and create a new design. Begin sketching on the XY plane and draw a rectangle of arbitrary diameter on the second quadrant. Then on the right hand side edge of the rectangle, draw a circle with centre at the midpoint of the right hand side edge. We will assign the dimensions once we have the basic shape.


Select the plane


Sketching on the plane


  1. We will now trim out the left half of the circle, by using the trim tool found under the trim drop down menu. Before that, we need to constrain the two shapes. We will constrain the circle as being a tangent to the corners of the rectangle. Do this by selecting the tangent option under constraints in the main menu.
  2. Assign the dimensions as given in the image below. Next, draw two concentric inner circles for the shaft; the first circle having a diameter of 3.5 mm and inner circle having diameter of 3.5- (2*0.3) = 2.9 mm, where 0.3 mm is the desired tolerance. We multiply it by 2 because for a circle, we need to consider the tolerance on both sides.


Drawing and dimensioning


  1. Extrude the entire geometry by selecting the extrude option or using keyboard shortcut ‘e’ and use the New body command, giving thickness of 3 mm. Next, extrude the shaft by selecting on the inner concentric circle and the rectangular face, to a thickness of 8 mm. You should now have a model that looks as shown below.




Shaft extrusion


  1. We will now mirror the extruded geometry. Make an offset plane on the circular shaft. The command is founder under the CONSTRUCT drop down menu.
  2. Then, under ‘CREATE’, select the mirror feature and mirror the geometry about the offset plane being the plane of reflection.  After mirroring, the mirrored half of the object isn’t combined to the original part. To do this, under’ MODIFY’ click on ‘Combine’ and select the two components to be combined. This completes the first part of the joint.


Mirror and Combine


  1. Now, under the ‘Browser’ the part will be listed as a body. However, we need to convert the body into a component, so as to create a joint.


Convert the body into a component


  1. We need to create the other half of the hinge next. We don’t need to create another sketch for this. Let us extrude the component accordingly to fit the other half of the joint, by using the previously made sketch. Hide the previously made component for now, found under the ‘Browser’.
  2. Select the geometry, not including the inner circle (not selecting this will result in a hole, which will mate with the shaft created in the previous part), and extrude to a distance of 10 mm using the ‘New Body’ operation.




  1. Extrude the face as shown in the image, with a distance of -3 mm to obtain the geometry as shown below. Finally, to get the same protruded geometry on the other side, we will create a midplane by selecting the faces on which the holes are made on either side.
  2. Mirror the side protrusion we created in the previous step about the midplane using the ‘Mirror’ command in the ‘CREATE’ drop down menu. You can now make the first component visible.






Make first component visible


Create component from bodies


Assembly and Fitment

Assembly is a feature in Fusion 360 that allows you to join two individual components to form a joint and also specify the type of joint that it is intended to be used as. Let us now assemble the two components.


Component assembly


  1. Under ‘MODIFY’ select ‘Move’ to first move the two components away from one another.
  2. The type of joint we will need here is called a revolute joint, meaning it will rotate about a given axis.
  3. Under ‘ASSEMBLE’, select Joint, and the motion type as ‘Revolute’.
  4. Next, select the components you would like to join together that will form the revolute joint.
  5. Select the midpoint of the hole in the first component, and the midpoint of the shaft in the second component. If the parts are designed correctly, you will see an animation of the second part revolving around the first.
  6. If the components merge and collapse in on each other against the laws of physics after the animation is done, we need to enable contact between the two. We will do that under the ‘ASSEMBLE’ drop down menu. First, using your mouse, select one of the components and move them apart, then under ‘ASSEMBLE’, select ‘Enable all contact’.
  7. After, this the two components will show correct physical properties and will not merge into one another.




  1. As before, to 3D print this component, select the entire component, making sure both are aligned horizontally, and convert it to an STL file.

With this, we have explored the basic concepts of design of movable components, assembly and fitment, and kinematic analysis to validate the working of a mechanism. In the next unit, we will delve into the details of how to get started with 3D printing the components you have designed.

We would love to see what you build out of these learnings!

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