We show you how to use the Rib and Web internal bracing tools to improve the strength of your 3D printed models.
For this month’s introduction to Fusion 360, we are going to demonstrate an easy way to get started with modelling real world objects by importing images into Fusion 360 and scaling them, allowing you to simply trace out a two-dimensional image that can be extruded into a fully 3D model. This will make it significantly easier to model complex everyday items with relative ease. We will also take a look at a couple of functions that will help you to design internal bracing into your 3D printed designs which will help you to create stronger enclosures.
MODELLING REAL WORLD ITEMS
In the very first installment of this beginner’s guide to Fusion 360, we created a simple radius gauge. This tool is designed to make getting a radius dimension extremely easy, as you simply press the tool against the object you’re modeling to get the desired dimension. This works with any radius that is included on the gauge, In our case, 3mm to 12mm. What do you do though if the radius is much bigger?
Take, for example, the Uni-T 120C multimeter. This multimeter has a somewhat complex shape to it. The meter has numerous buttons, a few different component shapes, and even the top and bottom curves of the meter both have an unknown radius. This means, getting started with the modelling process for this meter is a complex task. It’s possible to find a large radius like this using a couple of different processes.
The most accurate method is to use a compass, ruler, a sheet of paper, pencil and the object you are measuring the radius of.
In this method, you start with a rough estimate of the radius. In our case, we start at 80mm and draw the radius, seeing if the curvature of the traced item matched the object we were trying to replicate. If it’s not perfect, try again with a slightly higher or lower radius. Generally speaking, you can guesstimate the size fairly quick, usually within a few attempts.
Whilst this will produce consistent and fairly accurate dimensions, in our case, proving that both ends have a radius of 110mm isn’t exactly the most practical method, as it needs to be repeated for each curve/object. A much simpler, albeit, perhaps less accurate way to devise this dimension is to take a photo of the object you wish to model and to import it into Fusion 360. This way, you can scale the image to the correct dimensions and trace it. This method is many times more beneficial as it allows you to easily model complex shapes and objects by simply tracing their outline. This way, you don’t need to painstakingly try and measure or calculate every curve or feature on a device but rather you can simply trace around the lines.
All of this relies on the quality of the photo you have though. When you’re taking the photo of the object, you want to take your time and do your best to ensure that the camera and object you’re taking the picture of are as parallel as possible. This will ensure that there is as minimal parallax distortion as possible.
Using your Vernier calipers, measure out the general shape of the item. In our case, the dimensions are 110mm long x 58mm wide. We sketch these into Fusion 360, as we will need to scale the image to fit these dimensions.
Press ‘L’ on your keyboard to use the line drawing tool and select the plane you wish to work in. You can create a cross shape using the dimensions, as shown here.
Note: You want to centre these lines on the origin point as this will likely help later.
Import the photo you took of the object you want to model (We have made our multimeter image available for you to download from our website).
In the main menu, select the drop-down arrow of the insert button and select canvas. This will allow us to import the image we took earlier into Fusion360 and place it on the plane we are working on.
Once you have done this, you will notice that the image is significantly smaller than the guidelines we created earlier. This means we need to scale the image so that it matches the actual dimensions of the object. This is done using the positioning controls shown here.
These controls allow you to position, rotate and scale the image as needed. Our first step is to rotate the image so that it is as straight as possible. This will make it much easier to create the shape using the line tool. You can use the rotation slider tool from the positional controls or for much finer adjustments you can use the Z angle input of the canvas tool window.
The easiest way to level the image is to use the reference grid in Fusion 360 and a straight edge of the part you’re wanting to model. In our case, this is quite simple as the multimeter has large flat edges. We simply need to adjust the rotation of the image until the straight edge is aligned to the grid.
Once the image is as straight as possible, it’s time to scale it to the correct size. We find the easiest way to do this is to use the click and drag tool.
This will cause the image to scale in the x and y dimensions equally, and thus keep the proportions of the image correct. You want to scale the image so that it matches the measurements we entered in earlier. You can click and drag the centre square of the positioning icon, which will allow you to move the image to help centre it with the guidelines.
Once you’re done it should look something like this. Your image is now scaled to the actual size of the object you’re wanting to model. You can now start tracing around the object. This is an extremely useful process that you will no doubt use many times as it allows you to easily model very complex designs ranging from a smartphone to a car.
ADD STRENGTH TO 3D PRINTED ENCLOSURES
Rapid prototyping technology such as FDM 3D printing is the perfect tool for irrelatively designing enclosures, however, the enclosures are notoriously not as robust as enclosures constructed via common commercial processes, such as plastic injection molding. Some of this comes down to the layer by layer nature of FDM 3D printing, which means that the parts are created with weakness along the join of each layer, but this is only half of the issue. The reality is, most enclosures/3D printable designs available could easily have their strength increased by emulating some design features engineers use in commercial products.
THE RIB FUNCTION
A Rib is a structure that gives rigidity between two points by essentially bracing two faces together. These are commonly found in plastic injection molded parts where sideways strength is required such as in the case of this router enclosure.
These ribs significantly strengthen the enclosure, allowing it to be constructed with thin walls. In the case of this router, the ribs also help align the PCB.
To get started, let’s create a basic box shape in Fusion 360.
Create a new project and press ‘R’ on your keyboard to enter the rectangle drawing mode. Draw a rectangle 120mm x 50mm wide on the bottom plane.
Press ‘E’ on your keyboard to use the extrude tool to extrude the rectangle to 20mm. Let’s then add a 4mm chamfer to the four corners and the bottom edges, before hollowing out the box giving it 2mm thick walls. When you’re done, it should look like this. Note: Make sure you set the rectangle to have the centre point central to the shape.
This is just a basic box shape that we can use for demonstration purposes, so the dimensions are not of significant concern. There are many ways to create these structures in CAD programs, however, Fusion 360 has a unique tool specifically for it, aptly called rib. This tool allows you to easily create ribs of many different shapes, but for the purpose of this exercise, let’s replicate the ribs from the router enclosure.
To get a clear view of the enclosure, let’s create a cutaway section. To do this, find the inspect button in the main menu and click on the dropdown arrow, then click on section analysis.
Select the plane you want to have the cutaway on. For us, we want the ability to look perpendicular to the rib so we picked the y plane. You then set the cutaway so that we can see as much of the object as possible, and thus, are only hiding the minimum. Note: This does not affect the model in any way, we are simply changing the way we view the model.
With the cutaway done, we now want to create an offset plane that will allow us to start the rib from our chosen location. Click the dropdown arrow for the construct button found in the main menu and select offset plane.
Lets, create the rib 20mm from the far end. Since the box is 120mm long, this will mean our offset plane needs to be 40mm from the centre.
Note: If these dimensions are not correct for you, verify that you have set the origin point so the rectangle was centred when creating it.
From this plane, we can now draw our rib. Click the plane we just made and press ‘L’ on your keyboard to enter the line drawing tool. Draw out the required shape of the rib, however, you don’t need a closed shape in this case. All you need is the outer lines of the shape, the Rib tool does the rest. We simply copied the dimensions from the router enclosure and will provide the dimensions so you can follow along. Once you’re done, it should look like this.
Once done click on the dropdown arrow for the create button in the main menu and select the Rib tool. This tool will simply extrude the shape you created by the amount you specify.
Note: The router had ribs that were only 1mm thick. This would be too small to offer much strength to an FDM 3D printed enclosure. The general rule of thumb we use when creating enclosures is to set the minimum thickness of any component to three times the nozzle diameter. In most cases, 3D printers come standard with a 0.4mm nozzle, as such, we generally make our walls 1.2mm thick.
Since we are just modelling an existing rib structure, we will set our thickness to 1mm and press OK. This will create the rib 0.5mm in both directions. Now, this is a very simple example where you can use the pattern tool to repeat the feature a specific number of times across a dimension. You can, however, use this tool to create a huge number of different types of ribs. The only limitation is that it needs to be drawn as a single line.
THE WEB FUNCTION
Another very common method of increasing the rigidity of a plastic enclosure is the use of webbing to combine sections, as can be seen here with this keyboard enclosure.
This webbing is used to give large surfaces strength to reduce bending when pressure is applied. This allows engineers to use significantly less plastic when designing enclosures as the walls can be significantly thinner. The good news for us is that Fusion 360 has a tool built in to help with this too.
To get started, let’s use the same basic rectangle box from the rib experiment, but first, we need to remove all of the ribs. In the timeline in the bottom left corner, select all of the rib features, right mouse click, and select delete.
Like with the rib example, we need to create an offset plane that we can model from. Click the dropdown arrow for the construct button and select offset plane. Create a plane 6mm from the bottom of this model. This will mean that our webbing will be 4mm high from the bottom of the model as the model has a 2mm shell.
Press ‘L’ on your keyboard to enter the line drawing tool and create the pattern that you wish to strengthen the part with. For this example, we will create a plain old grid pattern.
As with the Rib command, this tool will extrude the single lines you have drawn into a three-dimensional object of a specific thickness and extend it until it reaches the next object. Once you have drawn the shape of the structure you want, exit the sketch. Click on the dropdown arrow for the sketch button in the main menu and select the Web tool.
All you need to do is select the thickness of the feature. We opted to go 1.2mm, which is equal to three times the nozzle diameter, which for us is the sweet spot for strength and time.
Note: Like with the Rib tool, you don’t need to be quite as boring as this. Have some fun with the process and create unique designs.
With these two functions, you will be able to make significantly stronger enclosures that use minimal plastic and are still pretty quick to print.
PART 1 - BEGINNERS GUIDE TO FUSION 360
PART 2 - CREATING CIRCULAR TEXTURED OBJECTS
PART 3 - BLENDING & SWEEPING
PART 4 - RENDERING TECHNIQUES
PART 5 - HELICAL SWEEP