3D Modelling 101

Class Resources Including Shade Template can be found here:

https://drive.google.com/file/d/1rBmWVRU6TygQhWzbKaLLcNn3DBgpGNu_/view?usp=sharing

Why Fusion 360?

It is a 3D CAD/CAM/CAE 3-in-1 software. You get the functionality needed for Design, Manufacturing, and Engineering all in one program instead of across multiple software.

It has an integrated cloud service so it can back up all of your save files and save iteration information directly to a server; making it easy for you to access your files from anywhere, as well as collaborate with others.

3D modeling and rendering is great for running stress tests and simulations prior to developing a project for real.

At the end, you should feel confident in designing simple files of your own.

User Interface

We will focus on the different parts of the user interface as we continue along the class but here is a rundown on what to expect in each area.

User Interface - Workspaces

Depending on your task at hand, you can change the type of workspace you are in. Doing so will change the interface to have the more relevant features more accessible.

In this class we will focus on the Design workspace but will have a brief visit in the Render workspace at the end.

User Interface - Design Workspace

Tool Bar

The top tool bar in this workspace is divided into 7 categories of actions, with the most common ones being featured as buttons. Additional features can be found by clicking on the dropdown arrows next to the section names.

Create – Generate 2D profiles/paths and 3D bodies

Modify – Modify the existing profiles/paths/bodies

Assemble – Join components together

Construct – Options to construct planes, axis, and points to generate sketches/bodies elsewhere than 0x, 0y, 0z.

Inspect – Renders measurement information in real time or hides measurement info

Insert – Insert a file to use a reference

Select – Default active tool if not using anything else.

Browser (also referred to as the Tree often times)

A lot of the file’s objects and properties can be found in the tree for easy referencing. This will become more important down the road but for the time being, you can minimize it by clicking on the double back arrow next to the word Browser.

Navigation and Views

If this is your first time navigating a 3D program, be prepared for some first-timer disorientation as it may take a while to get adjusted on how to maneuver around in 3D space.

First and foremost, Fusion 360 is oriented so that the X axis is left and right, Y axis is back and forth, and Z axis is up and down. This is easily confirmed by looking at the Navigation Cube in the top right corner.

You can quickly jump to different views by clicking on the sides of the cube or the little arrows that are visible.

If the cube becomes “mis-oriented” you can try right-clicking on the little home icon (only visible when you hover in that area) and Reset Front.

If you wish to manually navigate, you have a couple of options. The first method is to activate the navigational tools at the bottom of the window. This method tends to appeal more to first timers at it gives them more control until they get a hang of how maneuvering works in Fusion 360.

The first button is for Orbital view – you can rotate around the object to view at different angles.

The second is to Look at a particular side of an object.

The hand icon allows you to Pan your view – slide your view around to either focus on something, or focus on a different area of the workspace.

The magnifying glasses are each for their respective Zooms – in or out.

If you are more experienced with software like Fusion and are comfortable with moving around in 3D space, you can do everything almost exclusively with your mouse’s scroll wheel. (That’s right, it’s also a button.)

Roll Forward – Zoom In

Roll Backward – Zoom Out

Click and Drag – Pan

Shift Key + Click and Drag – Orbital View

Not only do you have navigational tools at the bottom, you also have View options.

Display Settings allow you to change how you want your object(s) to be displayed as. Most often you’ll change the Visual Style to suit your task at hand; viewing objects as solids, in wireframe, or a combination of both.

Grid & Snap Settings will allow you to toggle on and off snap and incremental move. You’ll probably leave both of those on all the time, but sometimes you just need to have a little bit more freedom in how you move.

You are able to adjust how the increments are set, as well as how your grid squares should be spaced.

If you’d like to be able to view your project at multiple angles simultaneously, Viewports will allow you to do that.

Turning it on will give you 4 windows; Top view, freestyle, Front View, and Right View. To set it back, just open up the menu again and switch back to single view. (You can also toggle this by using Shift + 1)

Timeline

The timeline might seem insignificant right now because we just opened up the software, but it will become a key section that you will refer to often as you work.

Eventually it will look something like this:

The timeline will eventually let you modify actions you have done in the past without having to undo your progress back to that stage.

So, if you’re worried about making mistakes or you want to tweak something that has already been done, don’t stress it, you can still make modifications without restarting.

Simple Sketch

As an intro to two/three of the most possibly used functions, you’ll make a simple box with varying levels of extrusions.

Sketching is one of the most used functions performed in Fusion 360 with extrusion following it to generate 3D bodies out of the 2D profiles. This first exercise will help you learn the two tools.

When you first click on Sketch, it will prompt you for which plane you wish to sketch on. We will be using the X/Y plane for this warmup.

Sketch a simple rectangular box (or press ‘r’ for rectangle), with 10mm(y), 30mm(x) for its dimensions.

When you have it, hit Finish Sketch to complete the action.

Select the 2D profile we just created and Extrude (‘e’ for Extrude) it by 10mm(z) for its height.

If you mess up while dragging or typing the value, you can always enter the number manually in the popup box that appears.

If the popup box is gone, go to the timeline and right-click on the action and go to Edit Feature to bring it back up at any time.

This next step you might not need to do often, but for the sake of showing you that it is possible, we’re going to smooth out the corners and edges so they’re more rounded. We do this by adding a Fillet to the block. Select the whole block and then hit Fillet (or ‘f’ for Fillet).

And we’ll just add a 1mm radius fillet to round off the edges.

Now this is where things get a bit tricky to follow as you will be sketching and extruding things, however they can only be done one feature at a time. Just do them one step at a time and you’ll get the groove of the routine.

Start by hitting Sketch and selecting the top face of the block. Sketch an 6mm circle on one third of the box using Center Diameter Circle (‘c’ for circle). Complete the sketch and then extrude it out by 5mm.

Make sure to end the sketch first otherwise you won’t be able to return to Design mode to utilize extrude.

Return to Sketch and add another 6mm circle in the middle of the box and extrude it inwards by -5mm. You should notice that the extrusion shows up as red as opposed to blue. This indicates that the extrusion is actually cutting the material rather than adding.

Sketch one last 6mm circle in the remaining third of the box and cut it completely through by adjusting the settings in the popup menu.

Rather than defining a numeric value, we can simply set the Extent to All and it will automatically stretch from the top face down to the bottom.

You should now have a block that looks something like this and hopefully have gotten the hang of switching between Sketch and Design mode.

Canvases/Importing Reference Material

Let’s get to work on prototyping a lamp. Save your current file if you want to keep it, and then start a new file.

You can import your own sketches as a reference by setting up canvases.

Insert > Canvas and then select the plane you wish to project the image onto.

For our project, we will use the X/Z plane.

You should see the reference image projected onto the plane we selected.

By default, the canvas should appear semi-transparent so you can still see and use the grid, but if it isn’t, adjust the transparency.

Do not worry about positioning the canvas at this time, we will fix it later after we calibrate it.

When a reference image is added, it won’t be to scale as Fusion won’t know what the dimensions are supposed to be.

Calibrate the canvas to scale by right-clicking on the canvas in the tree to the left and selecting Calibrate.

To establish the scale to calibrate to, select the two end points of the bottom edge of the image and enter in the intended value of distance (135mm in this case).

Once it has been properly calibrated, you can reposition the canvas so that the left and bottom edges line up with the axis lines for easier referencing.

You can do that by right-clicking on the canvas event and Edit Canvas.

Lampshade

With the canvas in place, we can start tracing the lampshade’s profile. You can use the Line tool to draw the bottom, left, and top edges.

Since you know the bottom edge dimension, you can just set it to 135mm after selecting the starting point and Fusion will do the rest.

The left edge line isn’t a nice integer so go ahead and round it to 195mm.

The top edge is the same case, you can round it 25mm.

The right edge is different because it is a curved edge.

Instead of using the Line tool, you will use the Spline tool. Trace the edge as closely as you can by adding a point every few steps. (You’ll want to turn off snap for this or you might not get the position you want.)

If you made an error, you can still move the Spline nodes around as well as adjust it using the handles that appear when you select a node. You can also delete nodes if you added too many (select and hit Del/Backspace).

Now that we have the 2D profile sketched, we will now generate a 3D body by Revolving. To revolve a profile, select the profile and then hit Revolve.

For settings we will want to make sure it is a Full revolve so it circles around completely. If ever working on something where you do want the revolve to be partial, you can manually define the angle.

This will create a solid 3D body by spinning the profile 360deg around.

We will have to hollow it out since lampshades typically aren’t solid blocks. To do this we will use Shell. Select the top and bottom faces to determine the direction the shell is to happen, and then set the thickness to 2.5mm.

Now that we have the 3D body of the lampshade, we can hide the reference canvas. If you look over in the tree, you’ll see each item has a little eye icon. Click on them to toggle visibility.

By now you may have made some errors along the way and you have been hitting CTRL + Z to undo your actions. Fusion 360 actually has a really great way to allow you to make revisions without having to undo all of the correct steps you have done. The timeline along the bottom tracks your events not only to provide a neat time-lapse of your work, but to allow you to make minor changes without having to undo all of your work to that point. To edit any event, right click on it and select Edit (depending on what kind of event it is, it will either say feature, or sketch, or form, etc.)

Before we call the lampshade done, we are going to add a hole to the left side of the lampshade, so we have a place to insert the arm into. Set your view to be on the left side of the lamp and sketch an 8mm hole.

Why sketch a hole and extrude it instead of using the Hole function?

Because the edge is curved, we use this method to ensure that the hole is straight through the object and not angled to match the curve.

Extrude the circle so it will cut through one side of the lampshade (careful not to set it straight through the whole lampshade though.)

That is all we will do for the lampshade for the time being. Save your progress.

Take a brain break; this was a lot of information to process so far.

Lamp Arm

To start the arm, we are going to start within the lampshade. Sketch a line from halfway through the lampshade to the outside and set the length to 25mm. Make this in alignment to the hole you created (if you have snapping on, this should be easy enough to do).

For the curved section, because they are two simple curves as opposed to multiple curves like the lampshade, we’re just going to use a 3-point Arc.

You can find this under Sketch > Arc > 3-point Arc.

Set the start point to the end of the straight line you generated and set the second point somewhere left of the lampshade but level it with the base of it.

Start the second arc at the end of the last one and place it somewhere below.

Manufacturing this arm would be a little difficult as is, so we’re going to add some fillets to smooth out the crooks. Activate Fillet and select the two affected paths. Set the radius of the fillet to one that looks smooth (I used 40mm in this case).

With the general skeleton of the arm sketched out, we can toggle the visibility of our lampshade, so it is not distracting/impeding our visuals for the arm.

We have the shape of our arm, but now we need the thickness. To do this, we will sketch the diameters of the outside and inside of the arm at the starting point of the arm.

We will Construct a plane to ensure we start at the right spot. Go ahead and Construct > Plane Along Path, select the starting segment, and set the distance to 0.

With a plane to draw on, sketch one circle with a diameter of 7mm and a second one with a diameter of 5mm. Finish the sketch and return to Design mode.

From here we are going to Sweep a profile along the path to generate a tube.

Select the ring between both circles and go to Sweep. Your profile should’ve now created a tube along the path you created earlier.

That’s all we will do for the arm for the time being, feel free to unhide your lampshade and save your progress.

Save Iterations:

A nice thing that Fusion 360 offers is the ability to leave a note with each save so you’ll know which version of the save you are looking at should you need to revert a file.

Lamp Base

For the lamp base, we will actually create this in a separate file. Create a new design and you should see that a new tab has appeared at the top. You can switch between projects easily from there.

Given the complex shape of the base, we will not be able to generate a 3D body using sketches like we did with the lampshade and arm. Instead, we will be sculpting a simple 3D mesh into the shape we want.

For sculpting, you will need to go to Create > Form or use the purple cube button. You’ll notice that the top buttons have changed. These buttons are exclusive to the Sculpting mode.

We are going to create a Box on the X/Y plane.

Drag out a square and set it to 25mm(x), 30mm(y), and 25mm (z). This will create a T-Spline model that we are able to modify face and edges.

Tips/Pointers:

You will want to make sure “Shaded with Hidden Edges” is toggled on for the rest of the sculpting steps or you’ll have some difficulties seeing the faces and edges.

Before going too far, make sure to turn Symmetry on. This will help immensely as Fusion will replicate your actions performed on one side onto the other. When you activate the symmetry tool, it will ask you to select where the division is happening so select these two faces.

You should see a green line appear to divide the block. Now whenever you select a face on one side, it will appear blue, and the mirrored face will appear greenish/yellow.

With that sorted, select Modify > Edit Form so we can modify the block.

We are going to want to pull the front faces to create a leg so hold Shift while clicking to select multiple faces/edges.

If you pull it as is, you’ll notice that it stretches the shape as opposed to generating new material. If you press the Alt key while dragging, you’ll be able to extrude faces instead of just stretching it.

Extrude them forward by 125mm and then pull (not extrude) them -75mm to the left and -50mm down.

Tips/Pointers:

Avoid hitting ‘enter’ after each number if you’re doing multiple steps. Doing so will end your Edit Form function and you’ll have to reactivate it. After typing the value, just click and drag on the next directional arrow and enter the value for that.

The center of the base is looking pretty chunky. You can move the center edge back to lessen the amount of material that sits in the center.

To easily select a loop of edges, you can hold Shift and double click to select a loop of faces or edges. For the base, you may have to do it twice as the front facing edges don’t seem to be included.

Drag the edge backwards and then lift to slim out the center.

For the third/back leg, we are going to select two the face and extrude them back -50mm and then drag them lower about -50mm.

If you look at the base from the side, you’ll notice that the back leg might not be leveled with the front legs. Using the grid as your reference, drag the back leg to match the level of the front legs.

Slim out the back leg by dragging the face towards itself. Alternatively you can also use the Y-scale rather than Y-translate, it should still be the same in this scenario.

With the general shape completed, we can clear the symmetry and hit complete sculpt.

For the next steps, it will be easier to have the base to sit at a height of 0z so move the body of the base so it looks like it is just sitting above the red axis line.

Save your progress so far.

Take another brain break; this was quite a bit of work done.

Components

Before we start assembling the components, the lamp base is still missing one thing: a hole to insert the arm into. What we will do is create a plane at an angle so we can generate a hole that will go through the base at an angle we determine and not just whatever angle the edge happens to be at.

Construct > Plane at an Angle.

We are going to have the plane pivot on the Y-axis so select that one.

Set the angle to -30deg.

Using that plane to sketch with, we are going to sketch an 8mm circle that lines up with the center of the base.

Extrude the circle so it cuts through the base.

Now the base is done. Make sure to save it and then return to your lampshade file.

Since we have a stretch of the arm dedicated to being the insert for the lampshade, we will also need one for the bottom to be the insert for the base. We are going to edit the sketch for the arm, and we can do this super easily by going to our edit history and right-clicking to Edit Feature.

Add a 25mm line at the bottom end and angle it to be 60deg.

Make sure to also add a fillet to it to smooth out the crook. I had mine set to 40.

Save the sketch and then Edit the Sweep even so it includes the new segment.

Once the arm looks good, you can right-click on the arm’s body in the tree and convert it to a component for assembly. Do the same with the lampshade. Make sure to name the components for easy referencing. You can double click on their name to rename.

With those two components good to go, we’re going to bring in the base for assembly. Import the base by opening up your Data panel and locating the base. It is most likely saved in Default Project.

Once you have located the file, right-click on it and have it added to the current drawing.

At this stage, you may want to save your progress so far.

Assembling

Now it is time to join the pieces together. If you have designed your arm to go straight out of your lampshade through the generated hole like I had this next step should be super easy. If you did not, you will have to see how joining is done between the arm and the base and apply the same logic to the arm and lampshade.

There are 2 modes of joining you may use. This first one is As-built Join which will combine the two components as they are without moving them.

Simply activate the tool and select the two involved components. You should be able to see an indicator appear on the lampshade to show that there is a joint.

The second mode of joining is regular Join (J) which we will use for the arm and base. Before we join these two however, because they are separated, it is best to Ground one of the components, so they don’t move unintentionally. In this case, let’s ground the base. You can do this by right clicking on the base in the tree and select Ground.

To join the lamp arm to the base, we are going to activate the Join tool and then select the center face of the arm’s end, and then select the midsection of the insert hole in the base.

As soon as you do, you should be able to see the arm moving towards the base.

It will also look like the lampshade didn’t move however the render only focuses on the involved components. The lampshade should follow the arm as joined as soon as you confirm the joining between the arm and base.

In terms of physical modelling, that concludes it for the lamp.

Customization

Let’s talk customization. This can be done at any stage of the modelling; however, I have left it at the end so I can customize all three pieces at the same time and see how they coordinate with each other.

Start by determining what material each component will be made with. You can do this by going to Modify > Physical Material. Find the material you want to use and drag and drop it onto the component.

I have used the following material:

Lamp Shade > Aluminum
Arm > Brass

Now with the base, because it is in a different file, you won’t be able to drag and change the material here. You can actually modify the independent file and then just update the information in the full file.

We will save that for later after we also change the appearance of the material.

To change the appearance, you can find the Appearance feature in the same menu as Physical Material before. It will bring up a catalogue just like materials and you can select different colour variations of the material for simulation.

I went with Anodized Rough - Blue for the Aluminum lampshade, and I left my brass arm as is.

Now you can go back to your base’s file and repeat the same steps.

Once done, we can update the base within the original file. You do so by right-clicking on the lamp base in the tree and select Choose Version. This should bring up a popup where you can choose the save versions of your lamp base. Select the one that has been customized.

Before we render, we’re going to hide our joints.

Rendering

Once you’re happy with your lamp’s appearance, we can render a photograph of your model.

Switch to the Render workspace for rendering options.

Position your view of your object for the most aesthetic photo you can take. Navigation is the same as you would in the Design workspace.

You can take a test image by clicking on Capture Image

Once you’re satisfied with the test image, you can do a higher resolution render. Most often you will stick with the default settings so no tinkering will happen here other than determining optimal resolution/size for the platform you intend to share the photo on.

Make sure to use Local Renderer. It is possible to render on the Cloud however that charges a service fee per render.

I also opt to set my Render Quality manually.

Hit Render when you’re done inputting your setting options. It will start to process and you can see it at the bottom of the screen in the Rendering Gallery.

What is Rendering?

Rendering is when the software generates a photo. Factoring in lighting arrangements and material textures, it will render it pixel by pixel until the image is completely formed. For most high-resolution renders, you should be able to see the textures of your object so clearly it looks the way it feels.

When done, you can click on it and it will open in a previewer. You can download the image file and do whatever you wish with it. Voila! That is the end of the class! Congratulations on your lamp sample!

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