Full design walkthrough

00:00

And now let's apply everything that we have learned onto a complete bottle design in a new and empty design file. Let's go to the front view, then move the scene down. Snap options are all turned on. The unit system is millimeters, and we're going to create our first sketch. The sketch is going to be very basic at the beginning because we only want to block out the overall proportions of our bottle.

00:29

And then I will show you the process how through extra sketching and 3D modeling, we're going to add all the details. To create a sketch, click on Sketch with the line command from the origin. I need to draw a line straight up. I have to zoom out a little bit so I can see 200 millimeters. Then click on the Z axis straight up and another line 40 millimeters to the top.

00:56

30 millimeters to the left horizontally, 40 down and 30 back. And at the bottom, I also draw a line 30 millimeters. Right click, right click, drop the line tool. In the Constraints settings, turn on Always Show Constraints and Always Show Dimensions. So in this exercise, then we can see the dimensions all the time. And at one point when we have too many dimensions, we can simply turn this off so we don't see all at the same time.

01:27

First you see here at this point, there are two coincident constraints. So this one is actually this vertical one. This is the constraint onto the Z axis. This vertical one I don't want, so I delete it. These lines are blue because they are not constrained, so they can move. Let's make them horizontal and vertical. And then this will be 30 millimeters.

01:56

This will be 40 millimeters. See, I'm adding the constraints, completely locking down the sketch and this will be 30. Now let me zoom in a little bit. I would like to have a nice S transition from the cap into the bottle. And then also down here, kind of like a nice quarter R.

02:25

The distance from the top to this straight line should be 40 millimeters. And then the same at the bottom. To visualize this first, I will do this. I'll draw myself here a line that is 40 millimeters. Then I draw a line and here another line. Right click, right click, drop this one, and then that should be 40.

02:54

That is 40. Now I see exactly where this line here should be. So this one. When to the top and to the bottom, I have this 40 millimeter distance. These lines, I don't need anymore. I just simply used a drawing method to show you kind of like what I was trying to do. And this line, will make horizontal vertically constrained.

03:25

And now I can figure out the distance. So I select this line and the central line. Then here, I would like to add a little bit of the distance dimension, and that should be 40 millimeters. These dots are blue because everything can still move around.

03:54

I can now go ahead, select these two dots, click on this icon in front of the number and then say vertical. See that is actually 40. And there, one more time. I did not give this line any length dimension because let's say I changed this one, you see then the line will update.

04:24

This all works good. By the way, this is a point where, for example, I would turn off all the show dimensions and actually constraints too, because that is all done. Now I can focus on these nice transitions.

04:40

We will go to the Spline tool and we will work with the control point version. Start at the bottom. That's easy. This is the start, this is the end. And to create a nice and smooth transition of the spline starting here sharply and then smoothly flowing in there, we need tangent to this line, at least one to two points. One point is G1.

05:09

and two points is G2. Think about G2 as for industrial design, really the way you want to do this to get really nice and smooth transitions. So I will click and then click. This is now G1. This is now G2. And then I can go to the end and click, right click, right click, and drop the spline tool.

05:40

These points, because the way how I drew them, they do have a constraint to this line. So they are actually constraint to the guideline. So the direction of this line. So I cannot move them left and right. I only can nicely move them up and down, which is exactly what I want. And with this, you can see, I can now sculpt how this curve is flowing.

06:11

Okay, beautiful. Let's go and take a look at the top. I would like to do the same. So from G0 to G1 to G2, and then this is G2, G1, G0. So 1, 2, 3, 3, 2, 1, and right click. Here that is set, that is set...

06:39

There I will, this curve, will make Tangent to that. You see now this point can only go up and down. And then this point I moved to somewhere else. Now it's snapped to that constraint. And also here, I can now go ahead and for example, use the grid to define or specify.

07:08

where I want those points to be. Let's do a quick study. Here's our cap. There's the Revolve. Here's the bottom. Here is the Revolve. And this looks pretty good. The transition down here feels nice. You see the curve continues the direction of the line and then gently bends over. Up here, this...

07:36

feels a little bit too harsh. So if I bring this to there, this to there, this feels better. But I have the feeling that this section is too flat. So this mid part. And this is now a point where, yes, I could solve this via sketching and try to find where these points have to be positioned to create a beautiful S-Groove.

08:05

And instead I will simply use the Loft command for that. So in this sketch, I will add here a horizontal line. Click Exit Sketch. Then maybe the easiest way is right click this Revolve command, delete it. And then we select this and that, and then do a Revolve. Then I select

08:33

this top face and this bottom face and call the Loft command. Both should be G2. You see here, continuity for the surface. There's G2 and G2. You see now how this is really nice. And also pay attention to the difference of the program. We can play a little bit with...

09:01

these values, you see how I'm moving these points around a little bit. Oh, interesting. I got very close to even what I sketched by hand. And with this control a little bit of that flow. Very good. So this curve, for example, now I remove, I don't need this anymore because with that Loft command, I get a really even start.

09:30

and transition. I think we agree on that. This is a much easier step.

09:38

So now we have the main study for the bottle and the cap. And now we can start thinking about how we are going to do the inside of everything. So for example, the neck of the bottle, and then how we core out the cap, et cetera.

10:05

Because we started with one initial sketch, we can start adding into that sketch. And because we use the cap to do a Loft, I can't really do very much with that cap right now because it might change then the Loft. So what I will do, this is body 1, I will delete this body. You see here now is the delete function. That is all good.

10:35

Because now we are going into the sketch and now we're going to redraw the detail for the neck and for the cap. The initial cap was really in this case, just a target for this Loft comment.

10:54

With the line command, I will start drawing a straight line up, 30, and then a horizontal line. These will be horizontally, vertically constrained. This will have a material thickness of 2 millimeters. There we are.

11:20

This here, 30 millimeters. So this is kind of like the cap and I can now draw in also what I need for the bottle. So for the neck that goes in, there we are. And also here, the distance, two millimeters because that is where the threading will go in.

11:47

So this revolved around this axis. That is the part that will go to our bottle. So now I can select all these parts and hit Union.

12:05

Since we are there, let's go ahead and add a Shell command, 2 millimeters.

12:22

Then we can select this one, go to this axis and create the Revolve. And if I zoom out a little bit, go to section view, here's the plane I would like to do the section view along. There we can see now how everything perfectly sits on it. That's really nice.

12:52

Very good.

12:58

In this sphere, for example, we can now go ahead and start adding the threading if we want to, or we could add a Refine Details, we could add the handle tip on top. So I would always try to kind of like structure your work step-by-step and keep the most complex tasks at the end. So for example, the threading is the

13:29

just the mechanical part at the end, I have the gap for it. So this is the thing I will do at the end. And what might make more sense now is to continue refining the bottle, for example, and also the handle. So let's work with the bottle first. We do have here very sharp edge, and I would like to round this one.

13:57

say by 10 millimeters. There we have it. But if I zoom in, there you see the material gets very thin. That is not really ideal. This is a problem for manufacturing and it's going to be very easy to solve in our case, because here's a Shell command and the fillet, I simply drag in front, sorry, on top of the Shell command.

14:27

And there, you see what happened. If I put the fillet after the Shell comment, you see that now we take this, if I go to the insert break point here, you see this is our solid piece, then we shell this and then we fillet this. Now, logically, when this goes in front of the shell, we have our solid piece, which we then fillet and then we shell that.

15:00

For this bottle, I also would like to have a nice kind of like depression on the left and the right side. So kind like when I hold it, I can put my thumb and index finger over it. And this is something where we can use the Sweep command very nicely for.

15:24

I will hide the sketch, I will make a new sketch, and then I draw myself somewhere a circle. So three centimeters, 30 millimeters, kind like as a scale reference. This is very good. And I will, with the Spline tool,

15:52

draw myself a shape like this. You see, and then I can push this a little bit further in. You see how with the circle, what I was trying to figure out. The circle I don't need anymore. Now this shape, I will now turn off the section view. I will Extrude left and right as a study first. So here's my symmetry command

16:23

for the Extrude. So symmetric, and then I Extrude. There we are. And I cut into my bottle. Again, we learned this is not really going to be a big problem. I just have to put the Shell command at the bottom. There, it's all done. Otherwise, if we go back to the section view, there you see how this worked out.

16:50

So with this sketch we have, we can then play with the shape, how far this goes in and ideate a little bit.

17:04

but now this is just only a straight extrusion. I would like this to go around this a little bit. So this overall idea is good, but I need to change my strategy a little bit. So what I will do is this sketch and this extrusion, I will delete. This was just a test. And then I go in front of the Shell command too.

17:34

So now when I start adding features, everything will be added in front of the Shell command.

17:41

I will go ahead and add a construction plane from the ground and click Next, and then offset this construction plane to a height, let's say 120. This construction plane is going to be very useful because on this construction plane, I can now attach a sketch.

18:11

We will use the Spline command for this. So one click there, one click there at the center, and then one click there. You see they're perfectly symmetrical and right click, right click, and then drop the Spline tool. I will move this point a little bit to the outside. So it starts to touch the bottle and then you see at the end, it feathers away.

18:43

Because I drew this sketch onto that construction plane, if I click that construction plane feature in the history, you move this up and down, you see how everything follows with it.

19:00

Along the Spline, I can now attach another construction plane. And when you select a sketch and then go to the toolbar, you see the suggestion is to add a construction plane that runs along the Spline, kind of like a roller coaster. I go to the midpoint, go to the side view, select this construction plane, click Sketch, and

19:30

Basically now I can do the same thing what I did before. Here is my helper. There we are. And then I can kind of like sketch this one out. There we are. Connect this, bring this in a little bit as much as desired.

19:56

Yeah, this feels good.

20:02

And now what I can do is I select this sketch profile, then shift left mouse button, select the Spline and Sweep it across it. And there you see, because the Spline does not follow circularly the cylinder, but touches it, but then feathers away, the shape intersects with the bottle the most at the center, and then it fades out.

20:33

We can do now the following. We select the bottle, then I select this part, click Subtract. And you see I'm removing from the bottle this part, click Done. So if I now go ahead and select this Spline and move this, you see how I'm moving

21:02

the shape, kind of like guiding it around that bottle.

21:08

Very nice. This looks good.

21:12

We could mirror over the sweat body to the other side to create the symmetry. We don't have to create the sketches at the same time. We can also mirror over the surface detail. That will be easier. I will add here a small fillet. There we are. And then I will select with the mouse those surfaces, click Mirror.

21:42

Select this mirror plane. You see how this is projected over, click Done. And there it got mirrored over. Now let's go to the front view, turn section view on, move this one down.

22:00

And then we see everything perfectly fits. This is nice.

22:12

At this point now, it will be good to continue detailing our cap a little bit. So I will delete this break point. Now we see our cap again. The bottle here, I will hide. It might also be good to start renaming our parts. This is the bottle. There we are. This here is our cap. We can also put

22:41

specific sketches and elements into folders.

22:48

I call this one Grip. So this way, the more objects you have, you put them into folders and it's easier to sort what you have. And this one here I will call Cap.

23:05

And we could call this main sketch model.

23:12

Wonderful. Very good.

23:16

So this cap, we would like to add a nice kind of like handle on top. And to do that, I will select the top face. Then I will go to the Extrude command and extrude this one up by 30 millimeters.

23:45

One quick section cut. Yep. That is quite a lot of material we can use to slice through. I will now go to a side view because I will show you how we can sculpt this cylinder into a really nice handle simply by using two sketches and the Extrude command. And then with the Fillet command, we will soften everything. This is kind of like working with foam when you

24:15

draw your profiles onto a foam cube side in front, and then you use a bandsaw. Pretty much the same process. I will zoom in a little bit and then I will turn on a sketch. I do see here my intersection points. This is where the bottom of my cap is, so I cannot go below that. And then with the Spline command, I start

24:45

somewhere there on top, click, and then I feather out to there.

24:56

right click, and then with a line, will go ahead, clean this one up and close this.

25:06

Then I have here the Z axis. If you do not have this, you could also draw a line. Let's say you didn't model it centered in your world, because with the Mirror command, now I can select these lines here and then select that axis and mirror this over. So when I adjust this, the other side will always follow it.

25:36

I will bring this one down. You see how we can play with this. The distance here should be 10 millimeters. That is good. We can go into a 3D view, exit sketch. Then I will select these two sketch profiles, go to Extrude, turn on the symmetric version and then cut this out there. Beautiful. That's good.

26:07

I will go to the right view, zoom out a little bit, go to section view, and you see this is the wrong version. Click on delete. And now I can select this view and zoom in a little bit. Because I think I can move this one down a little bit.

26:37

Maybe one higher. If you have a little bit more of material there on top. See the section tool is actually really, really useful. I will turn this one off. I will hide this one. I will go to the front view. I would like this to extend a little bit more. It turned out to be a tick too short. So I can go to the history and change this

27:06

add 10 more millimeters by making this 40. This also coincidentally, you see, I drew my sketch quite taller, so I do have space to extrude this one up. If this is extruded too much, then I would have to adjust my sketch. But you see, now working with the history and adjusting these modeling features is really very powerful.

27:34

I hope at this point, you start noticing you don't need to know everything when you start modeling. You can really in a very slow way, solve small problems and then step-by-step ideate and with the history and rearranging features, then you can also go back and restructure the logic of how you are approaching designing the spot or any design. Now we need in this front view, create the opening.

28:04

So I will in front view, quickly create a new sketch. I will use my Spline command there and there. Right mouse button, click, right mouse button, click these two points. I would like to be symmetrical to the Z axis. I will bring this a little bit further up.

28:33

Coincident constraint. So I will delete this one there.

28:41

And with that, I can bring this a little bit higher. I can bring this a little bit lower. You see how I'm controlling how much this is arced. This is actually the top part. And maybe this is what I will do first with this spline. I will split the top off. Think about this like a hot wire when you have a piece of foam and you hot wire cut. To do this, let's go to Tools, Split

29:10

this body split by this curve, done. And then here, this one we delete.

29:19

There. Then we can go back into editing the sketch. I would need to have an offset version of this. Can, with the Offset command in the sketch, create myself a nice copy of the sketch, 10 millimeters. You see the shape is the same, but we have more control points. This is normal. And now,

29:49

I can use the Spline command and then click here, down, there, there, there, and up, right mouse button, click, right mouse button, click. This all should be symmetry. So you see how I'm selecting these pairs. And with that,

30:17

Adjust all this. That is good. I do not want anything here on the spline to change, so I will lock it. And now I can very easily move things around here.

30:39

I do not want this one to go over. So you see here, we have this curve that goes to the right side. This should go to the right side. good. So this point you see here with this guideline, make sure that it is not on the left side. It should be right under it, or at least to the right side.

31:08

There, perfect. So by moving these points around, we can then ideate on the shape. Now I would like to cut this one out. And when you click here, you see I'm selecting the front faces. What I will do now is I will call the Extrude command and say Symmetric. And then here I

31:38

right click and say, select through at this point.

31:44

And you see it selected that part.

31:49

Or I say right click, select through at this point. You see, then I can select the profile. And now one more time, hold the Shift key, right mouse button and select through at this point, hold Shift and click this one. I have now both profiles selected. Now I switch Extrude and Symmetric and just cut through.

32:14

Beautiful, cool, okay.

32:19

I noticed that based on how I...

32:25

positioned everything here, I can pull these points further a little bit. maybe also a little bit, a little bit lower there.

32:46

It's just so beautiful how you can adjust the sketch. And then while you're in Sketch, you see the update on your 3D model and perfect everything. Very nice. This is good. To make everything nicer also on your hands, let's round these sharp edges, 10 millimeters. Here on the inside, you can select these edges and then we can

33:17

round this one too a little bit, not too big, a little bit like this. Also here we have the ability to switch to G2. So we get nicer changes. This is something I do very often at the end. I start working with G1 and then, because they are faster to calculate. And then when the design is done, then I can switch over to G2. So here,

33:46

These sketches, when I go to the feature, edit it, there you can see there's a slider for G2. If we go to the front view and take a look at the changes, you see how with G1, the surface comes up and then instantly comes to fillet. And with G2, it continues that direction and then it blends. It's just a softer transition.

34:17

We can select forward and backwards these pairs, very gently fillet those or quite big based on how much material we have left to fillet. And then here, I will select this and this to a very tiny fillet, one millimeter. And then here also I can do when everything

34:46

is nice, adjust those to G2. Let's go to the display mode and turn on visualized because now you can see then everything without these edges.

35:05

Looks really good. Let's go back to Shaded. Or you can also here turn Show Edges off. We also have hidden edges if you want to look inside.

35:23

When we show the bottle, you see we made very good progression. I would like to make a section cut now here from the front.

35:41

A little bit of cleanup. We can select these two sketches, make a new folder, rename this. We can call this Cap Detail.

35:56

There we are. And I would kind like say at this point, the overall styling of this bottle is nearly done. Maybe here we want to add a tiny fillet. So I, with the mouse, left mouse button, click, drag to the right side, and then I press tab and you see on top, there is a slider. I only want to select these two edges, and then I add a

36:27

half a millimeter of a fillet just to break this. This just looks really nice. You can clearly see, there is a separation of two different parts.

36:42

And because the overall styling and design of this bottle is done, this is not a moment where we have to think about how we can do the threading. So for the threading, I will go back into a section cut because it's just very useful. And the threading I will put into a new sketch. So we can create a new sketch. Here's our opening. You can work on the left or on the right side.

37:12

So let me show you how easy it is to attach a basic threading idea.

37:20

And I drew left and right these lines. So I can then onto these lines, draw myself some nice looking triangles. I want those triangles to have here a height of, let's say, three millimeters.

37:47

the same here, three millimeters. When I select them and say, be equal and the same here, equal, you notice how now this point is perfectly in the center. So when I zoom in and then draw a line and you see from there, that is 1.5, 1.5. Just a nice little trick. How you can use Smart

38:17

constraining to generate these types of clean geometric shapes. From the bottom, let's say the start's at two millimeters, and then we need to have a little bit of a spacing there in between. I make this threading a little bit bigger, so it is visually also easier to see when I start modeling.

38:45

The dimension here for the distance, I will select this point and this point, one millimeter. Because I wanted this to be a vertical distance. So my cap in my bottle, will turn off. I will also turn off the section view because now we can create our threading. You see also the height of how far we can do our threading. I will select

39:15

this inner triangle that is the threading for the bottle. Shift click then the axis, go to Revolve. And now we have a 360 degree revolve. Take a look at this one here. If I now go ahead and start moving this one up, there we have a threading.

39:45

We could do the same here. And then I move this one up.

39:53

5 millimeters now, and there you see how they are starting to interlock. Let's undo this and undo this one. Cause what is important now, we need to figure out when we do the threading. So we go with 5 millimeters. So that's for the distance. But how many turns do I want? So 360, let's say 4 turns, multiply by 4.

40:23

And now we will get an error message. That makes sense. So let's bring this one up a little bit and then say, multiply by four. Now we have four turns. And the reason why we got an error before was we would have created a self intersecting body. And the trick left now to do is, you see here is my

40:52

other threading. So I need to position this to 20. Remember the first turn was five, we made four turns. So five multiplied by four is 20. That's it. So with that, I know I can do this and then do a Revolve. I go up by 20 and then I say,

41:22

Multiply by 4.

41:26

See threading is actually really super easy in Shapr3D. The last step left is now to attach those to the individual correct bodies. So this one I double click, shift, double click, and then say Union. There we are. This sketch I would like to hide. We can then do exactly the same also to the cap. because

41:55

We have a direct modeling here. We can rotate those faces a little bit. You saw what I did. I just selected that face, selected with the mouse button and shift that edge, and then I just rotate it. So when these threading starts touch each other enough, they are not rubbing so much, they're more sliding. And then we could select these edges and start filleting them, for example. So please feel free to experiment there.

42:25

Then I will go and show this one and this, and let's do a Union. There we are. I could then go ahead also here, select this, bring this over.

42:45

Beautiful. And there.

42:52

The names of these parts can change. You see, this is body three. So let's rename this Model and then we will rename this one Cap. good. This we should rename into threading. This is really very good practice to sort everything because if you

43:20

step away from your design, you come back some weeks later, and then you only see body one, sketch one, names. It's very often difficult to understand what is what. Very nice. The last thing maybe to do is go to the visualization mode. I will give this bottle a nice car paint.

43:46

There, this is beautiful. And then I will make this powder coated or powder coated metal a nice.

44:01

kind of like a grayish color. And then for the cap, I can go to a plastic, maybe a matte, make this one nice and black. And then here with the environment, we can play around a little bit. This gradient mode is really nice. Make a gradient in the background. And then there we have a beautiful presentation

44:31

of our product and we can see how this could look.

44:39

And that's it. We built a beautiful bottle, including threadings and everything.