Explore a step-by-step guide on how to create 3D models in Fusion, including how to add vertical base, sketch directly on the 3D geometry, and create geometry in two directions. The article emphasizes on the importance of dimensioning and constraints, ways to make sketches easier to read, and methods to create distinct bodies in a model.
Key Insights
- The article provides a detailed process to create a 3D model in Fusion, emphasizing the necessity of dimensioning and constraining to avoid movement when clicked and dragged. It also explains how to toggle between real geometry and construction geometry.
- A crucial step in creating clear and readable sketches is to move dimensions around the screen, which, although not necessary, can significantly enhance the sketch's readability in the future.
- While creating geometry, the article highlights the process of creating geometry in two directions and ensuring that the operation is set to new body to maintain two distinct bodies in the model, which aids in creating a specific part in the future.
In this video, we will continue to work on our base. You will notice that I am still in the Step 01 Base file, and I am still active in my Base component.
The next thing I would like to do is to add the vertical part of my base here. We need to create a new sketch to create our 3D geometry, so let's go up into our toolbar and click Create Sketch. You will notice that our origin planes have once again appeared, but in this instance, I do not want to select one of my planes.
I would like to host my sketch directly on my 3D geometry. I will hover over my body here, and as I do, you will see the top face become a lighter color. I will click this top face, and you will notice that we reorient to that view.
As I navigate in three-dimensional space, you will see that it has projected my origin point, but to the top of this plane. I will go to the top view and rotate twice to reorient my view. So let's continue sketching.
I will go to the rectangle tool, and I'll draw a rectangle in the middle of my geometry here. Again, the size does not matter. We will dimension it now.
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I will press D for Dimension, select the top of my rectangle, move my mouse and click, and I will type 30, then press ENTER. Again, click the side of the rectangle, move your mouse, and click again, and this dimension will be 15, then press ENTER. We can see that our geometry is blue, so as I click and drag, I can move it around the screen.
I would like to place the midpoint of this rectangle somewhere around here, but I have no geometry to snap to. So let's draw a line using the line tool. Snap to this point and drag away into this space.
I would like to point out a few things about our line. As I click this endpoint, you can see that I can drag it anywhere around the screen. I would like to fix this, so I will go to my Perpendicular constraint, select my line, and then I will select the top edge of the rectangle, and you will see the line turn black with a white endpoint.
This means that the line is constrained, but the endpoint is not. So I can drag the endpoint up and down to change the length. Let's press D for Dimension, click my line, move my mouse away, and click again, and I will type 30.
Our line is now fully dimensioned and constrained, so it will not move when we click and drag. The only thing I would like to change about this line is that it is regular geometry in my sketch. I do not want this geometry to influence my future 3D modeling, so I will change it from regular geometry to Construction geometry.
That is done here in the Sketch palette by selecting the line and then selecting Construction, or selecting the line and hitting X on the keyboard. This will toggle the geometry from Construction geometry to regular geometry. You will notice that it has remained constrained and dimensioned, but it will now no longer influence our future 3D geometry.
Let's go to the Midpoint constraint one more time, and I will select this line and this endpoint. You'll see the triangle appear, which will show that we are using a Midpoint constraint, and all of our geometry has turned black. Now that our rectangle is in place, we can click and drag on any of our dimensions to move them around the screen to make our sketch a little bit more clean.
This is not a necessary step, but I like to do it to make my sketches easier to read in the future. I will hit Stop Sketch at the top of the screen, and again hit the Home icon in the ViewCube to reorient my view. Now we need to create our geometry, but first we need to cut a hole in this bottom geometry so that we can slide our new part in.
I will go to my Extrude tool and select this profile, and I will drag my arrow—rather than up to create Join geometry—I will drag it down to create Cut geometry. For now, I don't care about the distance.
Just make sure it goes through your entire geometry and hit OK. You can see that we have now created a hole in our geometry, and our sketch is automatically turned off. When you use a sketch in Fusion to create three-dimensional geometry, the sketch will automatically turn itself off after the first time you use it.
If I go to my Base component in the browser and hit the dropdown arrow, then go to Sketches, you can see that I can turn my sketches on and off whenever I need to. Go ahead and turn Sketch 2 on by clicking the light bulb so that the light bulb is yellow, and you can see your sketch on the screen. Now I will go to Extrude one more time, select this profile again, and I will drag up 60.
But as I drag up, I can see that I still need geometry to fill this hole. I will change my direction from One Side to Two Sides, and you will see a second arrow appear. I can now drag down with this arrow to create geometry in two directions.
I will make this distance 15, and before I hit OK, I need to check my Operation. We can see that the Operation is currently set to Join. If I hit OK right now, it would join my main body at the bottom and this vertical body into one body.
I do not want to do this because in the future, I may want to create this part separately, and I cannot create it using joined bodies. I will change this to New Body and hit OK. We can now see in our browser, if I open up the Bodies folder, we have two distinct bodies in our model.
I will hide Sketch 2 by clicking on the light bulb and again go to my Home view. In the next video, we will finish up our base by adding a hole here and fillets around the bottom of our base. Go ahead and save your model, and I’ll see you in the next video.
