Explore the process of modeling a lampshade in 3D, including the application of thickness to create solid geometry, using various constraints and functions such as the concentric constraint and the mirror command. Discover how to create threads for 3D printing, combine multiple bodies into one, and apply fillets to soften edges.
Key Insights
- The 'thicken' function used in 3D modeling adds a thickness to a surface to create solid geometry, transforming a 2D lampshade design into a 3D model.
- The 'mirror' command and the concentric constraint aid in creating identical bodies and aligning them perfectly with the original model, ensuring symmetry in the design.
- For 3D printing, features like threads are modeled and fillets are applied to soften the edges, enhancing the final printed product's functionality and appearance.
In this video we will apply a thickness to our lampshade and create the rest of the lampshade geometry. So let's get started.
I will scroll down and find step 8 and open it. Once your file is open you can go ahead and hide your data panel. And if I look at my lampshade component we can see that we only have a surface, no solid geometry.
I will activate my lampshade component and go to create, thicken. Thicken adds a thickness to a surface to create solid geometry. I will select my surface and zoom in and drag my arrow to the inside.
If I orbit to the bottom of my model you can see a thickness being applied to my lampshade. I will type in negative 3 and hit ENTER. We now have our solid geometry.
I can see in my lampshade component that Fusion has automatically hidden my surface and created solid geometry. Now I would like to add some extra bodies to my lampshade component. I will make these from Sketch Base Modeling.
%20(1).png)
Learn CAD
- Nationally accredited
- Create your own portfolio
- Free student software
- Learn at your convenience
- Authorized Autodesk training center
So let's go new sketch, zoom in and select this interface of my lampshade arm. You will see the model reorient itself and right now it is hard for me to see the interface of that lampshade arm because my lampshade is in the way. We can use slice in the sketch palette to cut a temporary section along our sketch plane.
If I check slice you will see the rest of my geometry be cut away in section and the bottom of my lampshade is still showing because it comes past the section plane but now I can easily create my sketch. The first thing I will do is to go P on my keyboard to bring up my project window and I will zoom in and select this inner circle. Next I will go circle by hitting C on the keyboard and I will draw a circle here.
Again I'm not worried about its position or size. We will constrain in dimension now. We are going to use a new constraint, the concentric constraint, which places one circle on top of another.
I will go concentric, select this circle and then this circle. You will see the concentric snap up here and my circle can now be resized but it cannot be moved. Let's go D for dimension, click my circle and let's type 20 enter.
All of my geometry is now either purple because it was projected or black meaning it's fully constrained and dimensioned. I can go ahead and hit stop sketch and notice when I hit stop sketch my temporary sliced section disappears. We now want to extrude this to the edge of our lampshade so I will go to extrude, select the profile.
I am not selecting the inner profile because I want to create a hole and on the extent I will change this to two object. Our lampshade is an organic form and I want this extrusion to touch it exactly. Now with my extent set to two object I will select the lampshade body.
We can see that our extrude is now going directly to the edge of the lampshade. I'll say new body and hit ok. We can now see in our lampshade component we have our main body and this extra body on the side.
If I want to create another copy of this body on this side I could use CTRL C CTRL V and move it into position. However it is much easier for me to use a mirror command. I will go up to create and find mirror.
I will select my pattern type to bodies and select either in the browser or the window body three. Next I'll select my mirror plane and I can select my origin plane. We will see a preview of my body appear and it in the correct position and I will hit ok.
Now that my bodies have been mirrored into the correct position I can right click isolate my lampshade component so that we can finish modeling without being distracted by the rest of our model. Now I would like to combine my three bodies into one body. I will go to modify combine and I can select all three of these bodies holding CTRL in the browser or dragging with a window around my bodies.
I will join my bodies and I do not want a new component and I do not want to keep my tools. I simply want these to be combined in the existing component. I will hit ok and now we can see we have one body that is completely combined and connected.
We only have a few other steps to complete our lampshade. The first is creating threads which will go in the holes on each side of our lampshade. I'll zoom in and go to create thread.
In fusion creating threads is as simple as selecting a cylindrical face. I will zoom in and select the inside face here and you will see a thread begin to generate. You will notice that this is just a visual thread it is not modeled.
Because I want to eventually take this lampshade to a 3D printer I would like a modeled thread. So I will go up to the thread dialog box and select modeled. You can now see that fusion is actively cutting away from my geometry and adding geometry to create a modeled thread.
I will keep it as full length and all of these other settings look appropriate. I'll change this to left hand so that it will attach to my bolt. Just be careful when setting your designation that it will eventually match your threads in the future.
I'll hit ok and orbit my model to repeat that process. I will go to create thread, select the inner face, select modeled, and again change this to left hand and go ok. Finally the last thing I would like to do is apply some fillets.
Fillets will soften the edges of our model and make it easier to 3D print. I'll orbit to the bottom of my model, go modify, fillet, and select this inner edge here. I don't want to fillet this too far, let's say 3mm, enter.
Next I'll apply a fillet to the inside edges here and here. So I'll go modify, fillet, and select these two edges and let's make this 2mm and hit ENTER. And again I can right click and drag straight up to repeat my fillet and I'll select this edge and this edge 0.5mm and hit ENTER.
Our lampshade has now been thickened into 3D geometry, thread connectors modeled on either side, and we've applied fillets to make rounded edges. I will collapse my lampshade component and activate my main component and right click un-isolate. Go ahead and save your file and I will see you in the next video.
