Soap Bottle | Modeling Projects

Hello everybody and welcome to this tutorial in which I'm going to show you how easy it is to sculpt such a nice looking organic soap bottle in Shapr3D. Topics we will take a look at is all the necessary sketches we have to only create and then how by using the history line, step by step, we are going to create the building blocks of our design and then use these very basic building blocks and start adding all the details, for example, edge roundings, inside shelling and fillets, build the piece outside, create then a functional cap and even, for example, use the ability to resume and suppress features to prototype various stages of how elements could be rotated and manipulated and then we will finish with a really nice looking product presentation, adding some colors to the background and materials for an adequate color material studies. And with all that said, let's do it. So here we are inside a new and empty design. The first thing we want to do is make sure all our snap options are turned on and also our unit system is set to millimeter. A bottle is a revolve body, so the easiest way to start is by going to the front and creating the front profile to revolve. I move the screen down a little bit, go to Sketch and we will start with the Line tool. At the center of the sketch where Z and X meet, I draw a line to the left side, select the first point that is the center of my bottle and hit the block icon because this point I never want to move. This line I will dimension to 30 millimeters, select the line and also constrain it to be horizontally aligned. I can zoom out a little bit, then I draw a line straight up. This line will be 150 millimeters and vertically constrained. Zoom out a little bit more. And then on top, I can draw a line to the left side. Make sure this is horizontally constrained and this is 15 millimeters. This is, for example, the top diameter and 30 is the bottom diameter and the 150 is the height of the body. Since we have the Line tool active, we can zoom in to the top and put in the preliminary geometry for the cap. This will be 40 millimeters up, horizontally constrained. Then I can go to the right side and go down and make sure that these two lines are horizontally, vertically constrained. So now, as you can see, I have 150 and I have 40 millimeters. To show the dimensions all the time, we can turn on always show the dimension, also always show the constraints, or leave this off. And then when we select the line, we see everything that is important. We can now go ahead and create the spline to sculpt the shape of our bottle. Go to the Spline icon, double-tap it, and then you have the option between the Control and the Fit Point. I'm going to use the Control one. So what I will do is from the top, I start drawing and then press, go down, press, go to the center and inwards, press, go down, outwards, press, go down, press, go to the end and release. And you see, this creates a really beautiful shape. What I can do now is play with the distance of how far these points are apart from each other. So here, I will make this a little bit smoother by bringing these points down so they all have exactly a similar distance to each other. On top, I would like to have a sharper corner. And also a nice and long part on the curve. So there you see the distance is actually much longer between these two points than these two points. And then with this one here in the center, I can play with how much this belly is in. And that, for example, is in the space where the fingers kind of like go around the bottle. At this point, we kind of like have everything to make a quick prototype. So we'll select in the sketch profile of the bottle, then select a vertical line with the Z-axis and click Revolve. This hides the sketch. So we can show the sketch one more time and then select the sketch profile again, select an axis and Revolve. Beautiful. That's good. What is actually really nice is we can actually then go ahead and select the sketch, go into sketch edit mode, select nothing. And then when we select individual points, we can move them around and see how this does update the shape of our bottle on the fly. That's actually really beautiful. Even while history-wise, the sketch is created in front. So before the Revolve bodies, we can edit steps at the beginning and see how this influences the rest of the construction in real time. This is super amazing. This bottle is very round and all I want is from the front to see this nice curvature look, but actually from the side should be more flat. So I need another sketch. I will go to the bottom. Then I will go to sketch. And you see, when I do this, I have all these sketch intersections to prevent, for example, any accidental snapping. I can turn everything off and then create the circle. So I don't snap to a piece of a sketch or geometry where they intersect. Very good. Change my view, rotate, exit the sketch. Then I can show everything. And you see that the sketch also sits actually directly at the bottom of the bottle. So you can just select the sketch and you see where it intersects with the bottle. This is a new profile to select. That's not really what I want. So what I will do is I will select the sketch, exit it and then simply move this down a little bit. How much is up to you. Beautiful. You see, now I have just one sketch profile. So let's select the sketch. Going back to the bottom view. And with the spline command, I can now go ahead and draw myself a nice curve. And there, beautiful. When these two splines are not connected via a symmetry constraint, I can model every spline basically independently. And if I would like the front and the back spline, kind of like function like a mirror, then I have to create a Y and an X symmetry. So let me show you how we can do this. This is very easy. So we'll select the line tool along the Y-axis. I make a line and along the X-axis, I make a line. I select both lines and lock them so they don't move. Now, select nothing. Then I select two pairs of points, symmetry and the X-axis. The opposite symmetry axis and the center points and this axis line. When I now select one point, you see the opposite moves. Pretty good. But you see here, when I go left and right, now the right point doesn't move. So this is actually now where we will select the left and right points, symmetry, and then we lock this to the other line. And then when we go ahead and move these corner points, there we are. Now I can go ahead and for example, move this one up, move this one down or stretch this out. And by this, essentially with this line, can project how I'm going to slice the bottle. So let's do this. We will exit the sketch. Select nothing. Select the sketch profile and then hit the up arrow, extrude. And then we cut through the bottle. Obviously, I don't want to remove the bottle. I want to actually remove the outside. So by clicking on this tiny icon with the white sphere and the blue cube, I can then get into the Boolean command and decide to add a union, new body, subtract. And actually, I would like to use the intersect command. And that basically gives me the volume of how these three objects, so the cap, the bottle, and the thing I extruded intersect. Again, one little tiny demo. When I go back to editing my sketches, I see everything in real time. It's actually really nice how this works. And the same is also true for this one here. I don't have to go even into a 2D view. I can prototype this by selecting the sketch, going to sketch, edit, and then I use the grid for the movement. There we are. So this looks actually pretty good. So we have the main bottle and the cap. We don't really have actually the neck that goes onto the bottle. And this is where I will go ahead and then select the first sketch we created and edit it and create two more lines that go inside. One line to here. This should be 11 millimeters and horizontally constrained. And then one line straight down, vertically constrained. And this line should be 30 millimeters. When I now open the history, you see I have my first sketch, my two revolutions, my second sketch, the extrusion. And when I click on the first revolution, there I see that this is actually the feature that created the main bottle. I click on the arrow on the right side to expand it. Here I have profile and axis. Click on edit for profile. And then I will add this sketch profile I just created to it. Click done. And I have updated my design. Notice actually how easy you can create different iterations and you start with very basic models. And then step by step, we create more refined, complex models. Let's refine this bottle. I will turn all the sketches off. So I only see this bottle. And I can pay attention to how these edges all meet. There are various different ways how we can fillet them and round them. We want also later to shell the inside. So before we do a shelling, we want to round all the sharp edges on the outside because in the shelling command does actually the work of the inside because the rounded edges will shrink down to the inside. And we'll see this in a moment. When I select this edge, just as a demo, just don't follow it, just take a look. You see how I can round this vertical edge. Then I get these nice rounded corners, edges, and then I can round this a second time. And then what you see is we get this connection where we have two profiles, which are rounded, and then this centerpiece. But we have here very sharp corners. That's not really very nicely looking. So I undo everything. We can select all edges at the same time. There we are. Then we drag the arrow to round this and pay attention to how this looks. This is nice. And then we click the clock icon and switch the corners from rolling ball to setback. Takes a moment to calculate and take a look at these beautiful corners. They look really great. We want to adjust the radius of the fillet. We can go to History, look where the fillet command is, click on the arrow to expand it, and then change the radius. There we are. It's very easy. We could also select a face of that fillet. And there you see it says Edit Fillet. When we click on this, then there we go back to the original command and here we can change that value. So same thing. So this is actually done. That's good. This corner we can keep sharp. That is fine. This one I would like to round a little bit. One millimeter. This looks sufficient. And now the bottle is ready to be shelled. So I can select the top face, go to Shell, and I will select two millimeters, which is a little bit thicker. I do this on purpose because it's an easier surface to see. If I go to the front view and then at the bottom left, select Section View, we can take a look into that space. And there we can see how we have also inside all the edges. See, that's the reason why we fillet the edges first. And then we do the shelling because it does create this for us in the inside with a perfect material thickness. I have here a very sharp edge. If I would like to round this, I could also round this fillet actually. Sorry, this edge, say by one millimeter. Let me show you something. I go to the History view. Here's my Shelling command. Here is that Fillet command. And if I press onto it, Hold, I can drag this in front of the Shelling. And there everything is updated. Pretty nice. This is actually a pretty big fillet. Change this a little bit. You see everything updates for us automatically. We can zoom out a little bit and then go to turning off the Section view. And there we are. So we have now the main bottle and the neck done. We don't have the threading. The threading is something we can do later. It's a complicated task. And this only makes sense when also the cap is done. So let's go ahead and prototype the cap a little bit. I will go to Items, Sketch 1 was the first one we created that has the basic dimension for the cap. Currently, the cap is only a cylinder. We would like to change this obviously now. Then let's go ahead and edit this cap. I would like to have a wall thickness of 2 millimeters for this cap. And the cap actually has a lid on top that can swivel. So I need to define now a vertical line here. So I draw one line down. I will actually also hide the geometry, so this is easier to work. You see, I drag the endpoints onto the edges, make sure this is vertically constrained. Then I can select these two lines and make sure this is 2 millimeters. We have a swivel. So here's actually the horizontal line. And this should be around 4 millimeters. Now when this cap rotates onto the neck, it should kind of like seal it a little bit. So I would like to have here a very thin horizontal cap or lid that goes over it. And then we cut a hole into it for the fluid to come out. And I need one additional horizontal line. And 1 millimeter. So if I zoom out a little bit and only select the elements for the cap, main body, that's this. This is actually the space where the threading goes in. This is a cavity. And then this is actually the part of the swivel, kind of like the button that can rotate to open and close. And as before, we can go to the history. In this case, it is Revolution 2. There we are. Open this, go to Add Profiles. And now I deselect everything, and then just select only what I want. That is it. Click OK. And there we are. Look, we have actually updated that geometry. So you see, we don't really create basic geometry and then make new ones. We actually build basic geometry and then we can start adding more elements to it. We can close this a little bit. There we are. We can then select this upper sketch profile and select this line and do a revolve. That, for example, is actually the part that can rotate. Just with a finger press, we move one side down and then the other side goes up. The interesting element now will be to prototype the mechanics. So this is a cylinder that sits inside an open cylinder. To rotate, this is not necessarily going to work this well. We might maybe need to change the thickness a little bit, or we can also round this a little bit. So this is actually going to be the rotation axis. So that dictates that from the front, when we go back to the sketch, turn off the section cut. Right here between these two points, this straight line needs to be changed a little bit. Kind of like it needs to be a little bit round. So we can do this very easy by turning everything off. So it's easier to see. Then I will go to the line arc command and create here an arc. There. And then this point, I simply drag over to this axis, because that is the revolve axis. And this tiny extra profile, I created this one. I need to add actually to the rotatable part for the revolve and also remove from the housing. So you can go ahead. Here we have actually two movement commands. I can press and hold and say delete. I don't need those. There we are. Very good. And there is this revolve command. I can go to profile and then I will add this one simply to it. Beautiful. There you see. And then from here, I would like this tiny element to be removed. Go edit and there, click on it. We'll select, deselect everything there. Just select this one then. And there we are. Perfect. And there you can see, we have that space for it. Really good. Beautiful. Now there will be actually in the front and opening and also in the inside, we will shell out. And for the rotation left and right, we do need some sort of a sphere or something, like a joint. If we use a sphere, that's very easy to do because we add it to it and then we can press this cap into the housing. So we can go back to our first sketch. There we are. And I kind of like see where this one is. And I will add this actually on the other side. Now you have to be careful how much material I have. So they're like two millimeters. And I will draw a circle roughly here. This might be height-wise okay. Select the center point and then I can move this out a little bit. There we are. Very good. And then here I draw a line straight up and straight down. Make sure these lines are horizontally, vertically constrained. Three millimeters. That is good. And I will now hide this body and select the sketch profile, select the axis and hit Revolve. Now I have actually one, kind of like one joint. This element, I would like to mirror over to the other side. So I select the three dots, expand the menu, select Mirror, keep Originals on, and select this mirror plane. There we are. Perfect. Then I can now show actually all three bodies. So the two spheres and also the cap and join them together. I move actually the sketches closer to each other, so it's easier to select them all. There we are. The inside, at this point now we can shell out. I will do this. With a 1.5 millimeter. That's a little bit easier also to see. A more realistic value, for example, would be one millimeter. And then we have these folds here, the leftovers that shell and come out. Not a big deal. Simply select them and then we press Delete. And then that cleans it up. Now, because we added actually the spheres to the cap, we don't have that yet inside our housing. It's not a big deal. We can simply remove it. So from this one, so from the housing, I would like to remove the cap. Select, Subtract. So you see, I double-clicked actually both bodies. And then to keep Originals, we want to keep the removed body. We can actually rename these parts, for example, so it makes more sense and it's easier to find. It's a suggestion I can give you. And now there you can see how we have actually these openings. Now, because these are spheres, you can all see it. It's going to be very easy to just simply force press that into it. Beautiful. Okay, so we're making good progress. The next step is we can prototype how we can rotate the part and then where the opening is. So let's see how much we even can rotate this one. When we double-click this, and because this is actually just 4 millimeters, the center of rotation is right at the center there. Perfect. Which means I can rotate this. So this is 15 millimeters. That's actually the max. 10, 12, no, 10 millimeters, 12 millimeters. Sorry, degrees of rotation. That will work actually pretty, pretty well. Go to the side view, select nothing, section cut. Now there we can see how nicely this seals. Pretty good. Okay, so 10 millimeters, sorry, degrees. Go to the history, we have no movement command because I hit actually the undo button. What I will do now is I would like to take this surface and shave off the back area at 10 degrees. Section view off. How do we do this? Super easy. Let's just create a new add plane. You see at the top face, select it, and I just create this plane. Don't move it. Select the plane. And then I just rotate this one by 10 degrees. And with this plane, I can actually now double-select the housing cylinder, select the plane, select split body, click okay. And then this piece, which we split, I remove. There we are. This plane, I will drag down in height. We don't really need this anymore to see, but we can understand now when we rotate this 10 degrees, how this perfectly lines up. And because the housing is only cut at 10 degrees, I can't press the button more in. There goes a lot more engineering into such a simple cap. I'm just simplifying the design here a little bit. Let's undo the movement command because I don't want this to be the timeline. Very good. Since we're working on the housing here, let's go ahead and detail this a little bit. We can give this a nice fillet, 20 millimeters, so it's nice and big. That is good. And also here, we can add a hole. The opening will be where I'm kind of like pressing my finger. So when I go to select sketch, we're creating a sketch right onto that plane. There is a cylinder and somewhere here, I can create a 4-millimeter cylinder and cut through. Now this is kind of like the opening through which then the soap will flow out. I go to a side view, select nothing, go to section cut, show actually the bottle and there you see, nearly there where it should be. I just need to move this a little bit over. Not a big deal. We go to sketch 3, select it, then we're in edit mode, select nothing, just select the point, and then we can drag this along the grid to the left. Beautiful. And we see the update of the parametric model in real time. This is actually really nice. This can go down and besides the missing threading, this model actually right now is done. So let's take a look at the cap. How do we do the opening? We can go to the front view, turn off section cut, then we make a new sketch. Actually turning section cut on now is very helpful because we see where the top area is. And go to rectangle, tap twice, select from center, and then along from the Z-axis, I make here a rectangle 5 millimeters horizontally, 2 millimeters up, double tap, horizontal vertically constraint. And then I can move this one up. Ideally, yeah, right under the top surface. There we are. Section cut off, exit sketch, select the sketch profile, and then we just extrude and cut through. We have very sharp corners. That doesn't look very appealing. We would like to round this. That's very easy to do. We just select these corners and round them a little bit, 0.5. Very nice. If we show the other element, so the housing for the cap, and then double tap our element, rotate it, and there we can see how this can come out. What about 12 millimeters? And what about 13 degrees? I mean, not millimeters. Sorry for this. This actually looks pretty good. Now this one does not really match. Again, easy fix. We go to our history. Here's my construction plane. There's my rotation. This was 10 degrees. And we just add three more to it. Need to figure out the direction. So I inverted the value from positive to negative. And there now this is perfectly matched. And this movement rotation command, when I hold onto it, I can suppress. Then basically it's turned off, and I can unsuppress and then show it. So I don't have to all the time rotate this lid element forward and backwards. I can simply turn on off the rotation command. In terms of modeling, we're actually now at the stage where we can take a look at the threading. I will create a new sketch. What is really nice is because we make a new sketch that cuts right through this body, you see all the intersection lines and points. For example, here, there's one and there's one. I'm drawing these lines down. And then for the moment, I'm turning all the bodies off. So it's easier to see. Zoom in. The distance is 2 millimeters. So I draw a horizontal line, horizontally constrained, then a line diagonally down at a height of 2 millimeters. And that is actually the wrong direction. This one I will bring down a little bit. So you see I'm prototyping my threading. So this is actually the threading that goes onto the bottleneck. And this is then the contact surface where it will touch with the threading of the cap. And that is actually going to be there. Also 2 millimeters. And then I can move this whole thing up and down to be nice and clean. I can specify this to be at 2 millimeters. There we are. Perfect. So let's make the threading for the bottleneck. Select the triangular sketch profile. Select the axis. Then we go Revolve. I am still in section view, so turn this off. And here comes the fun part. I'm just rotating this down, for example, by 4. So I have a nice distance. But it's only one turn. 360 degrees multiplied by 2 is 720. We get an error because then it would intersect. So let's go 8 millimeters down. 720. And there we are. That looks actually really nice. Turn this sketch on again. Then we select the opposite profile. Select the Revolve axis. Revolve. Bring this down also here by 8. 720. And there we see now how this perfectly lines up. Beautiful. Cool. So this is actually the threading for the bottle. Here's my bottle. I will select these two sketches and bring them down a little bit. I can actually clean this up now and drag everything onto one element. So it puts everything into a folder. Very nice. And the start and end of this threading is a little bit brutal. What's an easy way to fix this? Well, we can select one cap face, then select a vertical edge. And then we simply rotate that face 50 degrees. We can do the same with the other one. There we are. Now that already looks much, much better. Here would actually then be this inside edge, and this goes in by 50 degrees. And here, this one to there. Beautiful. And these rotations I did are also registered as rotation around axis features and can be adjusted afterwards all the time. So the reason why I actually created this is now I can select these upper edges and very nicely round those. So there's a much better looking fillet. And then the threading has a really nice start. I might want to do the same also for the other edges. So I can go to History, activate the fillet, go Edit, and then rotate my view and add the other edges of the other threading. Click Done. There. This makes really a lot of sense to work nice and clean and group your command. There we are. Beautiful. So that's threading. We will join to the bottle by simply double tapping each body and then select Union. Very nice. And then we do the same with the housing for the cap. Union and there. Very good. So there we are now. To bring everything to an end, we can add nice fillets to our specific edges we can select. For example, all those and round those a little bit. Have to be careful that the value we're selecting is good. There was actually a small collide properly up here. This is nice and good. These tiny fillets are actually really nice because they make everything look nice and soft. And also when we create visualizations, they create very nice separations between the body parts because they create like highlights and shadows. And simply you see where pieces are put together or not. Let's unsurprise this one. This looks very good. So everything is now ready to go into the visualization mode. So I go to Modeling, select Visualization. There we are. And we can now decide what type of material here we would like to use. We have Glossy ABS, we have a Matte ABS. We can drag the Matte ABS of the main body and then the Glossy onto the top. Then the Glossy I also put onto the rotation element. You see the other material was then removed. That's a red bottle. Let's streamline this a little bit. So the Matte material I would like to be instead of red, simply white. So tapping onto it gives me then the ability to select a white material. And then the Glossy one, since this is going to be for a bathroom application, I give this a nice kind of like a nice mint color. So there we are. So we can just pick something here. They're beautiful. This looks good. And the white body does not separate really well from the background. That's a very easy fix. We just go to Environment. Here we have various options of default background, transparent background, a colored background. And because this is a colored background, we can click on the cog. And then also here, for example, give this different materials. And now you see, based on how we work on, do we make actually the cap pop more? Do we make the background pop more? We just play with the color contrast. There we are. Then we have the ability with the rotation for the light to specify where the shadow is and also where the highlight is. If the material for the cap, for example, is way too glossy, it's a very easy fix. So we look down, we have, for example, PVC or melamine. We can simply select the glossy material. And at the bottom, we changed the color of the material. But on top, you see, it says to the right of ABS, change. Select it. And then we can swap this out and select different types of materials. Now this actually works really, really well. Very good. That's how easy you can do very quickly a nice CMF study of your product and then theme everything based on the material and then also the color. And then to create a nice rendering or photo of this, all we have to do is click capture. And that is everything in this video. I hope you saw how easy it is to create such an organically sculpted body and then also how easy it is to create threading and prototype. A mechanical cap. Have a good day.