Floor fan

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Hello everybody, and welcome to the Shapr3D tutorial, in which I'm going to show you how

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we can build this nice looking floor fan. In this exercise, I will show you

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how we will start with a very basic set of sketches to build our basic building blocks,

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design our product, and then use the history and Shapr3D's new history-based

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parametric modeling, how we can adjust all the individual modeling steps we did

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to build this design, to perfectly perfect it. And with all that said, let's do it.

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So here we are inside a new empty design. Before we get started, let's make sure our snapping

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elements are turned on and the unit system is set to centimeters. I will go to the front view, move

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the screen down a little bit, create a sketch, and then at the bottom, draw a line to the left side.

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That should be 15 centimeters. The starting point I will lock so it doesn't move. And this Base,

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I will make horizontally constrained, so it doesn't rotate. Then I draw a line straight

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up. You see this one is slightly rotated, not a big deal. Let's go to vertically constrained.

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Makes sure it does not rotate left or right, but goes straight up. This line will be 79 centimeters

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long. Zoom out a little bit. There we are. We can continue working on the top. So here at the end,

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I will draw a line to the left side, make this 6.5 centimeters long and horizontally constrained. And

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then I just draw a line down again. Don't worry if you draw your line slightly crooked. With the

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constraints, we can correct everything. Very often I sketch profiles very quickly and then I use the

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constraints to perfect them. Here we draw at the bottom, also a horizontal line and constrain it.

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And then this long line will be 66 centimeters long. So we kind of like have actually the fan

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body. Let's finish the fan base. I can draw a line and I can draw a line and I can draw a line. And

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on purpose, I very quickly sketched these out a little bit crudely, just to show you how powerful

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the constraint system is. All vertical lines I select and make horizontally constrained. The

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first one here is 10 centimeters long and the smaller one is 1 centimeter long. There we are.

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And then this line automatically gets rotated accordingly. Perfect. So now we have the top

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and the base ready. We can exit the sketch, select the sketch profile of the base, select a vertical

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edge and do a revolve. The first sketch is hidden. Let's show this again. Select the sketch profile,

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select a vertical line and do a revolve again. Now we have a pretty nice looking cylinder sitting

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on a cylindrical base. Now we can... Imagine this one can rotate very easily and that's a

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nice solid piece. Now we can work on where the air outflow will be. To make work a little bit easier,

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I will hide body 2 and 1. Create a new sketch and then somewhere draw two vertical lines. I

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select both, make them vertically constrained. I also make them equal. So the same one line. I can

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select and dimension to be 40 centimeters. Then with an arc motion, I draw two arcs,

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top and bottom, select an arc, select a line and make them tangent. So the lines and arcs flow

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tangently nicely into each other. And then when I select the radius, it should be three. So we have

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a diameter of 6 centimeters. We can clearly see that this is floating somewhere in space,

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and I will use the Z axis as a snapping position. So now it's nicely left and right centered.

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And to have more control of where, for example, the bottom and the top edge will be, I can go

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ahead. click on Project, and then select from the first sketch, the top and the bottom line,

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and project them into the second sketch. If I had the first one, now you can see actually the

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top and the bottom Magenta lines, and these are projected edges. I can't move them around. They

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are projected in. So when I adjust the first sketch, then these magenta lines will move. And

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what's actually really nice about this is I can draw here two vertical lines. These lines, I will

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make a construction line. And really important, I will make them vertically constrained. Now,

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if I go back to sketch one, you will see that this is half of a sketch. So the center line here,

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that is really where the center of my cylinder is. So in Sketch 2, this construction line is

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perfectly centered, meaning that actually this profile is perfectly centered. Now I can click on

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these lines and then take a look at how long they are. I can make this 12 centimeters and this is

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14. Let's make this 13 centimeters. Well, 13, both lines are the same, which means actually that this

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element is perfectly centered on our cylinder. So, with the sketch profile selected. Let's move

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this one out. You see that actually I moved this one out while not seeing body 2. I can turn on

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body 2 and this is a little bit too far moved out. Let's open the history. There's extrusion.

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Click on the extrusion feature and you see we can now go ahead and move this back. 8 centimeters,

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that looks actually pretty good. Perfect. So this was actually a nice quick example to show you how

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powerful the history is when we have to adjust a model after we actually created it. The top part,

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I would like to rotate a little bit. Now this is a revolved body because of the sketch,

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the top surface is flat. Not a big deal. Select the surface, go to the Move Rotate

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command because this is circular. It's the widget is positioned at the center of this

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circular shape or disc. And then we rotate this to 15. Degrees. Beautiful. Very nice. This is good.

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this body and the main body will be joined. So a union. So we select both, double tap on the face,

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select the whole body, and then we select Boolean Union. Now this, as you can see,

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is actually just one body. I know actually for manufacturing purpose, we will have a base

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and we have a top, and then we have a front shell and we have a back shell. So that means somewhere

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on top and somewhere on the bottom, I also need to, at one point, split everything a little bit

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apart. So I will hide the base. I will go then select the bottom face, go to Add Plane and move

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this plane. 6 centimeters, 4 centimeters up. Very good. The problem with the top is it is rotated.

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So do we do. It's actually very easy. We simply go back in time. With my finger, I press and hold the

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Move Rotate command on a Mac and PC. It's right mouse button and insert a break point. And then

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here actually have to move this on top. Should have been after the extrusion. And then there,

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I can add a construction plane. and I go down 4 centimeters. And then this break point I can

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delete. So now we can see where the break point was inserted. We can clean up the design nicely

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by moving, for example, both offset planes next to each other. So inside our history, we see cleanly

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how we worked. Also here again, when we click on the commands, we can adjust them. So I will

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move this one two down and the other one I moved two up. So in relationship to the air outflow,

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they are evenly spaced. This is actually pretty good. Perfect. So we do have actually now the

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ability to explore the rounding. Do we round this completely? This looks actually really nice, five

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centimeters. So we have a bigger flare on top and then the bottom. Click on the clock and go to G2.

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When we lower this value, there you can see how we add then a smaller radius to it. Now this is up to

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the preference how we would like this to work out. This is actually the top arc is circular.

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So this is G1, which means I can actually simply go back to the edge continuity on the history,

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select this to be G1 and then explore also here, the amount of... the radius and what type of shape

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I would get. Now this looks actually pretty good. I'm satisfied with that. So again, you see now,

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you modeled something and then you use the history to perfect actually your design. We'll quickly

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explore how does this look, how does that look. Everything is looking pretty good.

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So we know this will, we will open because there the air comes out. Here in the back,

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we will have to cut slots. So this is actually now the moment where we will start the shelling.

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Ideally, you want to do the shelling after we did the filleting, because if we can see that

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even in the inside, we have a beautiful offset of the outside surface. Very good. So that one

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is done. We can also select the main body, select this construction plane and say Split.

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Select the bottom part, construction plane and select Split. And these two split planes,

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I don't necessarily need anymore. Oops, that was the wrong button. I'm sorry. There we are.

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These two planes, we don't need anymore. So I put them... into a folder. sea planes

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and hide them. But with the split, what I did was separating the top and the bottom from this

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design. It's very useful later when we're creating the mating parts. Now, because this is shelled,

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we can work on the air's opening in the back because air has to be sucked in and then it's

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being pushed out. There are various ways how you can do this. We can create a sketch from the side

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or from the back. I will use the back for a very simple reason. We have Sketch 2, and Sketch 2

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basically shows me the top and the bottom maximum distance of where I want the air to go in. So

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I'm making a new sketch. Then I will do a project of these two lines. for example, and that actually

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would project then everything left and right. So I know exactly in the sketch where the part is,

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and then we'll do another project of the top part. There we are. And to make things easier,

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I'm going to hide sketch 2. Beautiful. So now you see like where's my air outflow. in the sketch and

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I can work on where I'm going to suck in the air. I will draw a line horizontally, and then I will

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select the line and the arc and say, tangent. You see that moved actually the line right onto it.

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Using the grid, it's actually really nice to work left and right nice and clean without the

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need of any complicated symmetry lines. I can turn on the visibility of this body so I can

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see how long this is, 10 centimeters. Now that's good. And then I draw a line down, over and back

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up. So I make a small rectangle. These projected lines were helpers. So we make them a construction

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line. select everything and say, horizontally, vertically constrained, so they can't move. I

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could constrain everything even more. I don't necessarily have to. Now with this piece done.

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I will extrude this one outwards. There you see how it intersects with the part. And this is a one

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centimeter line. So when I select these horizontal edges and round them with 0.5 centimeter, I get

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nice and beautiful circular ends. I can select the whole body, double tap. I want to have multiple

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cuts. That's an easy task for the pattern. So I go to the pattern tool. We use linear.

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Spacing is actually perfect. Then I drag this one down. For the spacing, we can now, we have a one

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centimeter opening. Maybe we will have a 1.5 spacing, so five millimeters. in between, and

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then we will add more copies. So 30 is not enough, 34. tick too much, 33. There we are. Perfect.

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Very good. Again, because everything is parametrically, we can go back to the features and

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adjust it. 32 will be even better. You see this move this a little bit up. Here, this opening is

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right inside the opening on the front. So I might be able to even just go with 30. So there you can

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see how I'm building everything. There. Very good. Okay, very nice. Good. Now, this whole pattern,

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I can select, move up and down, reposition it. I can also select my main body, then select the

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folder linear pattern 01 with all the parts inside and click Subtract. And you see then this way,

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it's a very fast way to select multiple objects. Body 2 is my target. and then linear patterns,

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there are one folder, are my tools. I do not want to keep anything, click Done. And we have these

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amazing cuts done. Beautiful. Really nice. This looks top. Let's take a look. Oh, this all fields.

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So we prototyped the air intake. We also have an air outtake. The problem there is we have nothing

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that really prevents any accident, like fingers going in. Because we have this flat surface,

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we can select it and then right on that plane of that surface, create a sketch. Here I have two

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intersection points. I can draw those. And that is 5.6 centimeters. There are different ways how

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we now can approach this. One really nice way is working with the pattern, or working with

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the sketch to create equal elements. I will draw one line down, go over and go up. And this... I

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will make 2 millimeters, so 0.2 centimeters. And inside the sketch, I can select these three lines,

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and then use the pattern tool to, at the moment, prototype how this actually would look. There we

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are. I realized I made a tiny mistake. This line is actually not perfectly... centered. So I will

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do the following. This line was good. I will draw a line to the left and the right, horizontally

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constrained. Then I make this equally constrained and say this should be 0.2. There we are. And then

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I draw a line straight up. There we are. And then this center line that we make a construction. So

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we have a central line and then left and right, we have now this element here. One second.

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Let me not select anything. There we are. Let's go back to the sketch and we will do now exactly the

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same. We will select these three edges and then we can use the Pattern tool to explore how this could

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look. So we will have an outside. a piece, then that's a little bit shorter. And then we have kind

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of like where I'm tapping there, and there. Nice and equal openings. So this is actually pretty

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good. So the pattern to the left and pattern to the right, that will work. I will not do the

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pattern in the sketch. This was really more an element to work actually with the piece. And...

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I will hide all these elements here. I just only want to see the sketch. going to edit mode. Try

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to close the sketch. This one here, I can make a construction line and then draw a line there.

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It is actually perfectly close now. So this construction line is more kind of like a

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horizontal, like a central element, similar to this line. Very good. Now, this piece. has

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to go into the body. Now as you can see, this is where it is. Can go to a side view, drag this in,

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turn on the section cut. And now there we can see how far this went in, turn on the history and...

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Maybe we make this 1.5 centimeters. Then this I move up a little bit. This lower face, I move

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down a little bit. There we are. And now we do the pattern. front view, double tap face, select all

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piece, go to pattern. and one centimeter for the spacing. That is perfect. Very good. And before I

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actually mirror everything over, I want to perfect how this will be flush to that surface. So you

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see, I'm selecting each face and then select the surface and say, Replace face. Also here,

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I will do it even while it intersects with that surface. It's a super nice tool to match surfaces.

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And I only do this on one side. And when that is done, then I will go over to the other side. Now

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here and there and replace face. There we are. Perfect. So these two I now can select. And then,

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because we work symmetrically, I will use the Mirror command and mirror this over,

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kind of like the Y axis. There we are. And the linear pattern folder and all the parts in it,

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and body too. we will do a union. And then here, the folders we can remove. And to help our design,

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let's clean up and put all the sketches into one folder. Let's take a look at what we have. There,

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that looks pretty nice, no? Good. We can currently see through the design, the interior elements are

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missing. That's not really a big problem. All we need to do is go to... Let's sketch one. There we

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are. And I will do a quick revolve body. Then this piece, we will shrink down a little bit in the

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diameter, and then we will also shrink this one down along the vertical height. Move this body out

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of this folder. There we are. Now there we can see, and there's something inside. Again here,

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this is our first offset, sorry, face offset, correct. And we can make this a little bit bigger,

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so it covers more of the interior geometry. Very good. Now these are pre-made mechanical parts.

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We don't have to model those. The shelling, the casing goes outside. That's different. So this

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is actually nicely done. I did not shell actually the bottom yet. I will shell this later when we're

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going to do all the fillet roundings, because this is something I would like to round and then shell.

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So the inside is also correct. Knowing this, this is a step I will do all at the end. So the base,

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we wait for later. I would like to very quickly create a nice hand grip right here. So side view,

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new sketch. There we are. We can draw a line 3.5 centimeters to the left, then 1.5 centimeter

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down, a little bit at an angle align. There we are. This is actually really good. And I'm going

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to hide all my parts, because this I will extrude by 8 centimeters one side, then I make this 16

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centimeters. and round also these edges, half a centimeter. This way, I'm not going to interfere

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with these bodies. Super easy. So the reason why I built this one is the following. I will select

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my top part. I will select this new body, and then I say, Intersect. Just show me that intersection.

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And you see, I will actually get... just a shelled surface, but actually there I want to have a

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volume, kind of like what the blue part is, but only the blue part inside this cylinder. So let me

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show you something. That's actually pretty cool. What I recently learned, if you select a body,

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and then if you select a face, can be flat or curved, then you can split a body by a curved

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surface. This part now we can delete. This one we will hide. There we see now we have the thing that

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was inside. So it's kind of like the intersect idea. We use two millimeters for the shelling. So

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this rounded surface, I will select, shell it by two millimeters. There we are. Pretty cool, huh?

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So let's go back to here. but I did not really cut open that space where the piece has to go in. Not

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a big deal. So I will go to the Delete feature, insert and a break point. And then from this body,

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double click, I will subtract this body, but I want my removed body to remain. And then I remove

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the break point. and the shelling here breaks, not a big deal. Just select the original face fixed.

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And then these two pieces, we simply fuse together via the join command. Go to the side view. So

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right and go section cut. And look at this. This is beautiful. This works really good. Okay. Very

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nice. We are slowly reaching a point where we also have to talk about fillets and splitting. So the

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top part is split and the bottom part is split off. Let's split this main body because it has to

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be a front and a back shell. We simply can select the main body, double click it, then go to split.

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body and because again, everything is symmetrical, we can do that via. kind of like this plane. So

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the XenX plane. Let's move this apart. Yeah, there we are. Perfect. That looks really good.

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This is the top. At one point, it makes sense to really give all your parts names. So this is

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front. This is back. bottom. This is the base. And this is kind of like the fan cylinder in the

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inside. I'm going to hide this for the moment. Okay, beautiful. I also would like not only

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to have these two shells kind of like sitting next to each other, but slightly intersecting,

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kind of like a lip function. And also to the top and the bottom. So I'm going to select the

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top one, go isolate. and I will select this flat surface, that's round, go to Sketch, then I will

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use the Offset command and from the inside or the outside, select an edge, 1mm. Perfect. And

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then here, I will move this one up by... 0.5 of a centimeter so five millimeters beautiful

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Isolate off, top one we turn off. There is this other sketch again. And then here

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now I can go ahead and say, so, hey, you, please extrude five millimeters

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up. Also this one I hide. And then here we add this five millimeter lip to it.

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Beautiful, no? So you see the top will very neatly just sit on that. This is how easy actually this

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type of work is. Now then we can select the bottom part. And here pretty much it's exactly the same

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process. Select the top surface, go to Sketch, and then Offset. Select either the inside or the

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outside. Select an edge, make the sketch. And then here, we select a sketch profile and cut into it

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by 5mm. Show the sketch and then to one part, we add it to... And then we do the same to the other

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part. I would like to point out all these steps again, they are calculated and captured. So I can

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adjust the initial material reduction or removal, and then I can also work on the addition of

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material. I can see all these values here, minus five, minus five, minus five. So if everything

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should be three millimeters, I just change these 0.5 to 0.3. Okay, so that was done. Let's hide

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this. We have here the sketches, move those in there. This actually I bring to the bottom. The

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fan, I will bring also to the bottom. It's the least important object. Now we can also talk

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about how does this go to the left and the right. That's actually also pretty easy. So we work with

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a sketch. Again, there we are, new sketch. And from this point here, so there I draw a line down.

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So this is linked, and just drag this one down and down and down. And then I connect it to the

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correct point. and exit the sketch. And we cannot decide. This is actually the piece we

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are going to extrude, but this cannot be extruded because this is a revolved surface. We have the

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sketch selected. Here's our axis. Again, I work very symmetrical. I can just select it, revolve

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it. And then we decide by how many degrees? 5 degrees. Perfect. You, we mirror over to the

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other side. Perfect. And then you and you, and you, we can join. To make things a tick easier,

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I will go the opposite way. First, I will say from this body, I would like these two to be removed.

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It's simply an easier math problem to solve. keep my removed bodies. Thank you. So there you see,

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that is done. And then I go to the front and then here I say all this, join together. There,

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look at this. There, beautiful. Maybe five degree is a tick too much. So here's the Revolve command.

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Two degrees. Look at this, so beautifully this was updated. This looks easier because it's a

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revolved, it's a circular surface. It's not parallel faces. So with this slight overlap,

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this will be easier to snap these two shells horizontally into each other. Very, very good.

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We can at this point think about filleting and rounding edges. I will work at the base because

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it didn't really work there much yet. So this I would like to be one centimeter. That looks very

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good. And then this I will round by 0.5, which is way too much. 0.25. That is better. I'm going to

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isolate this one and say this one 0.1. So 0.5, 0.25, 0.1. And now I can select the bottom part

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and shell it. 0.2. There you see it. Now all the faces in the inside are shelled too. Here,

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I have no option to say, so this one is filleted, and I have the Fillet command from that here. I

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can keep it this way, or I will go and say, Add it. And with the pencil, I will click and drag

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over this and add more to it. You see now, the other part is rounded too. Here I have multiple

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edges that need filleting. So, drag right to left, select only edges, and then probably here too.

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There we are. Rotate, that looks all really good. And then the top. Careful how far you go in and

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what you overlap, but this all looks really nice. 0.1. There are some blending issues. Sometimes

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it's also easier to just go step by step. I have to be careful with the pieces you select. 0.1. Oh

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yeah, I understand actually the mistake I made. This is actually 0.1. A 0.1 is actually very,

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very aggressive. 0.01, that actually would have been nicer. Little mistake,

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but I fixed it. I keep sometimes these mistakes I make also in the videos. So you see also I make

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mistakes and I can show you how I will fix it. So same deal here, like we did before. I go to this

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one beautiful view and then go to Edit, click and drag and add more edges to it. And there

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you see how this all grows really well. And which edge here is missing? I think the one at the

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bottom here. There, clicked it. Perfect. Pretty nice. Since we worked on this midsection part,

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we can isolate this one. The easiest way to only select the outer edges is I will go to the top

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view. Click and drag, only edges, only the outside ones now, because the others might actually,

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as they are, part of the other fillets. So I deselect this. And then also here, 0.1. Actually,

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zero one. They're nicely rounded. And if this is actually too small, well,

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we can go ahead now and say 0.05. Make this bigger. This actually does not have the lip,

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so we might even go with 0.1. Now we see like half of the material thickness is filleted. Again,

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I think this is a really great example to show you how powerful the history is. The top will

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be nice. I would like to have here a little bit of a bigger edge rounding, but I will run

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into the following problem. If I round this too much, we will cut into... our interior material,

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you see this now. So this fillet, I might have to actually move after I rotated this edge. The

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fillets I created here were finishing touches. This is actually more really part of the design.

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So if I go to the history, I can see, move, rotate 01. That is actually the face rotation.

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I can give this a name. So I inside the history can actually see it. There it is. this fillet,

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I will move right after I did this face rotation there. And there you see the inside is nice and

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rounded. That's how you can just then reorganize your history to create exactly the type of bodies

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and designs you want. Last thing we need to do now is actually create an interface. So I will select

47:47

this surface, then I will add a construction plane, move this a little bit away, because

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I can select this edge and project it onto this construction plane. This construction plane,

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I don't need anymore. Where do we have the sea planes? there, hide this. And in here,

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I can now go ahead and create. one circle, another circle, and another circle. All three circles

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should be equal. 1.5 centimeters. I do have, because of the projection, the center point.

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Take a look at what I'm doing here right now. I'm drawing a nice triangle and all these lines,

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I'm going to make. a construction line, then this long line will be vertically, this will

49:08

be horizontally, and these two will be equal. So now I have my sketch symmetry. So if I select one

49:19

circle and move this around, you see how the other one follows it. So I can play with, bring this one

49:30

down to here, and I select these two circles, go to Project, and then I select the face below. In

49:49

here, I would like to project as edge only on face. So I'm cutting actually the face. which

49:58

means I have no individual elements where I could create, for example, a button into it, different

50:07

material. I can very easily move this down just by a notch. I meant a notch, not so much. there.

50:30

There we are. round those or fillet those. So there's a very tiny surface depression. The

50:43

user can feel that there is actually an interface element. And inside the sketch, I will create left

50:55

and right, for example, a plus icon and a minus icon. For this, I will use the center sketch. From

51:06

the center, I sketch this one out, 0.6. 0.2, very good. Then we do the same here, 0.6 and... 0.2 for

51:24

the height. We need one more. 0.2 and 0.6. Here we will add one circle and then... another circle,

51:57

click the wrong tool. There we are. Also material thickness, kind of like 2 millimeters. And then

52:08

here we will add our rectangle, 0.2 and 0.6. And thanks to the grid here, I will decide

52:25

along the grid, I drew two lines. And with these lines, I will trim everything. Now I use the Trim

52:37

command and remove everything what I don't need. There, beautiful. Okay, now I can select here all

52:52

this. Now the rest are construction lines, so they don't really influence anything. This is

53:00

actually normal geometry. So for sketch geometry, that's different. Project. And there. Actually,

53:18

hold on. Let's go to the Project command. I think I clicked the wrong sequence. So this,

53:27

I would like to project onto there. Perfect. Sorry, I made one more mistake. This actually

53:39

should not be a sketch that's projected, but should be a face, kind of like cut into here.

53:53

there. That is what I wanted. Then when you adjust the sketch afterwards, also the projection, the

54:17

face slicing result will update too. So to bring this all to an end, we can select the sketches

54:27

here, bring this to there. This is all done. Now we can see how this could look and how this could

54:35

function. Let's turn on the fan body and go to the visualization tool. Our default material, that's

54:45

kind of like what everything is modeled with. I will select and say this should be this rather

54:51

rough. ABS material. We can adjust the color. Now everything has the same color. The body inside

55:04

for the fan, that one I make darker, so we have a better contrast. This looks good. And then I need

55:13

to click exactly where our interface elements are. a little bit of Click Sudoku, and these we

55:28

can give the new emission material. The emission material is pretty nice because it allows you to

55:34

give buttons a color and it has a light bloom effect. Let's go to the materials. This is our,

55:46

not materials, the environment. We can play with the light rotation. Yeah, this looks really nice.

55:58

Perfect. And there we are. Now we rebuild actually this nice

56:03

looking floor fan in Shapr3D with the new History-Based Parametric Modeling system.