Sooner or later, you're going to run into the limitations of 3D printed plastic. It's a great material for lots of different uses, but mechanical connections are not on that list.
Luckily, it's easy to find accurate 3D models of manufactured hardware, like nuts and bolts, and integrate them into your designs. In this lesson, we're going to learn how to do just that.
This class aims to help you develop the skills you need to make whatever you want. We're using the bike fender as an example project to teach you skills and tools that are useful for lots of different things.
Take the skills taught here, and make any project you like.
The whole point of 3D modeling is that it allows you to make a complete preview of your design in three dimensions without wasting any real materials. You can go as deep as you want into the details before you make the finished product. In this design, I’ll be using metal fasteners to attach the fender to the seat post, so I need to integrate them into the design.
Before I go any further, I’m going to create the split in the sleeve that will allow the clamp to be slipped onto the seat post. I do this by creating a sketch that will make a 2mm gap along the centerline of the clamp.
Data Panel > Upload
McMaster Carr is an industrial supplier with an insane array of tools, materials, and hardware. Their entire catalog is online, and most of the hardware has a perfect 3D replica available for download. You can design your whole project in 3D, use McMaster’s 3D models, and order the parts in small amounts directly from them when your design is dialed in.
I need machine screws and hex nuts for my project, so I go to that section on the McMaster website. I go with M-4 sized metric socket cap screws (I think that size and type will work well). 20mm seems like a good length to start with.
*Remember, everything in Fusion exists on the cloud, so when you import a model, you have to upload it.
I open the screw model and use the Measure tool under the Inspect menu to find out what the diameter of the screw shaft is. It’s 4mm (M4 screw… duh…). The diameter of the cap is 7mm.
Now I need to integrate these dimensions into the new features on my clamp. I create a sketch in the ZY plane and project the end of the clamp as a starting point. I offset a few lines to guide the rest of the sketch and complete the rectangle as a way to control the geometry. I use the 3-Tangent Circle to create a rounded edge at the end of the clamp feature, then use that circle’s center point to make the profile of the screw hole with another circle. I go with 4.1mm for the hole to give the screw some wiggle room. I also add circles at 7.1mm for the screw caps.
After trimming the lines to make the profile I want, I create an extrusion using the Join operation to start the geometry of the clamp feature. I extrude it symmetrically with a value of 12mm because the overall length of the screw is 24mm.
I create a sketch on the top plane of the clamp part, then draw two lines parallel to the gap in the clamp. I use this new profile to extrude + cut the gap I need in through the clamp feature I just made.
Next, I project the circles that represent the outside diameter of the screw cap onto a sketch on the side of the clamp feature. Having measured the screw cap, I extrude to a depth of -4mm.
To add the screw model to my design, I right click on the model and choose “Insert into Current Design”. This brings in a link to the file and lets me place it.
I go to Modify > Align and click the circular edge on the end of the screw cap, then click the outside edge of the circle on the clamp feature. This is a quick way to place the model exactly where it belongs.
With the screws in place, I insert the nut component and align it to the end of the screw. I change the View Style to Wireframe so I can see the edges of the nut through the clamp feature. I want the nut’s face to be parallel to the end of the clamp, so I rotate the nut 20º.
After copying the nut to the second screw location, I create a sketch on the side of the clamp and project two of the points at the nut corners.
Using these points, I create an Edge Polygon under the Sketch menu. This lets me create a 6-sided polygon by clicking the two points I just projected. I repeat this operation on the lower nut to give me the second nut profile. I offset both of these profiles with Loop checked in the offset window to create a pocket with a bit of wiggle room.
With these profiles in place, I select them and use the extrude tool to create the pockets. I change the Extents to “To”, then hit the down arrow with the cursor over the back of the nut until the back of the nut is highlighted. After clicking, I turn off the screws and nuts so that the extrusion only cuts the clamp feature.
Finally, I create another screw / nut receiver feature on the back end of the clamp so that I can make a very secure connection onto the seat post.
Now that you know how to bring hardware models into your Fusion design, download some hardware and integrate it into your design. Start with something simple like nuts and bolts, and as you get more comfortable branch out a bit.
The models are so well done that you can actually create mechanical joints between different parts. You can bring in a hinge, create a rotational joint between the two halves, and watch it swing in real time!
Share a photo of your finished project with the class!
Nice work! You've completed the class project