3D Printing Ball & Socket Joint on Fusion 360
Fusion 360 is a very good piece of software as it can be used to design a huge variety of objects to be 3D printed. If at any point I wanted to change my measurements, you simple click along the commands list along the bottom left of the screen until you find the original drawing. When you double click, it allows you to go back and change any incorrect measurements and then it'll automatically update the rest of your sketch.
I decided to use Fusion 360 to 3D print a ball and socket joint for my stop motion animation armature. I started by creating a new component, which is done by right clicking on the top of the drop down list to the left of the screen. This was named ‘Ball and Socket’. Then, I created a new sketch and used the centre circle to draw out the initial ball. The size of this will depend on the size of the armature joint. I then off-set this circle with another circle around the outside, which was 2mm. This will be the space between the ball and socket joint which will allow the ball to move freely. Then again I off-set another circle out from the original centre circle (as you cannot off-set an off-set), by 1cm. This is the socket. Using the centre square tool, I then drew a rectangle going all the way through the circles and out the either end. This will be the piece in which the joint will glue to the wire armature. It could be hollowed out using the hollow tool so that wire can be slotted in and glued into place. The length of this rectangle again depends on the size in which you want to the joint. The width should be no less then 1cm as this would weaken the joint. I then added a line through the centre of the entire rectangle which will be the axis of the revolve. Another line was then added from top to bottom through the ball and socket circles. This line needs to be over the half way line as it will be where the socket cup will end. Once all these sketches were completed, I stopped sketched and could then start to make the drawing three-dimensional. Using the search tool (’s’ on the keyboard), I search for the revolve tool. I then selected the outer socket section which included the rectangle joint, outer circle and the little outer circle piece that was the other side of the centre line. For the axis, I selected the centre line which was added parallel through the rectangle. This means that the 2D drawing, will revolve around the axis to create a 3D cup socket.
To do the same for the ball, I used the same technique with the revolve tool but this time only selected the inner circle pieces. Firstly I turned on the sketch so that I could see all the original lines of my drawing. Again, I revolved the selected pieces around the centre axis line.
Finally, I needed to add the gaps in the socket which will allow the joint to move at a 90° angle. This was done by firstly by creating a new contraction pane adjacent to the ball and socket joint. I pulled the pane out slightly so that what I was about to draw wasn't going to be directly onto what I’d already created. By moving onto front view, I could see exactly how wide this gap needed to be to allow the joint to fit within. Using the centre square, I started drawing from the beginning of the socket cup edge. I then drew out a rectangle that was 4mm wider than my joint. To calculate this figure automatically, I typed in the width of the existing joint (for example 1cm) and then added the ‘+’ symbol to add an additional 4mm (“1cm + 4mm”). The length of the rectangle was roughly half way through the cup. After drawing this, I stopped sketch and extruded the rectangle back all the way through the entire ball and socket sketch. In the extrusion information box to the right hand side of the screen, I clicked on ‘Objects to Cut’ and deselected body 2 which is the ball. This means that the rectangle will only be cut out of the socket cup.
This would be a perfectly functioning joint, however to make the movements smoother, I used the fillet tool to round off the sharp edges. When the ball joint moves into the 90° angle, it will slip into the gap easier as there aren't any sharp corners for it to get stuck on.
To test the joint works, I started by making the two bodies (the ball and the socket) into components by right clicking over the bodies in the drop down column to the left hand side, and selecting ‘create new component’. These were named appropriately. I then used the search function to look up the as-built joint tool which will allow me move the socket as if it was built and being used. I selected both components, making sure to say that the ball is the revolve. To ensure the socket cup wouldn't move around, I right clicked on the socket component from the left hand column, and set it to ‘ground’. To make sure that all the connecting bodies worked, I went to ‘assemble’ and ‘enable all contact’. This means that the ball joint will not pass through the socket cup but instead will stop when it hits the edge.
If the socket gets printed and the ball doesn't move smoothly within the cup socket, then I am able to go back to my original drawings and edit the measurements
