For our second project, we're going to design and model a bottle lock based on my instructable from 2014. It's a simple object, but it has two parts and a hinge, so it'll be good practice for working with mechanical joints and more complex forms.

Tolerances are also going to come into play here. The bottle lock will be made of two interlocking halves, so we need to figure out the right tolerance to let them swivel around a hinge.

Step 1: Create a 3D Model of a Bottle

Original Bottle Lock

To create a bottle lock that fits properly, I need an accurate model of the bottle. I use the measurements I got with my calipers to create all the profiles I’ll need to create a bottle.

First, I open Fusion 360 and make sure the units in my automatically created "Untitled" design are set to millimeters.

Construct > Offset Plane > Enter distance

Offset additional planes based on measurements

Sketch > Create Sketch > Select Plane > Draw Circle

Draw additional circles based on measurements

I start by creating a series of construction planes the correct distance apart that I can use to draw the circular profiles on. This is easy because I have all the measurements. I start by selecting the Offset Plane tool in the Construct menu, then I use the origin plane as my reference.

Q: How am I repeating the last command so quickly in the video?

A: Right-click anywhere on the screen and "Repeat X" appears at the top of the popup menu.

The length of the bottle neck is 48mm, so I offset the first plane by that much. I repeat this command and offset each new plane by the correct length according to my measurements.

With each of my planes in place, I create a sketch on each one and draw a circle with the correct diameter representing each part of the bottle that I measured. With these finished I have all the geometry I need to create the bottle.

Q: How am I getting the circles centered on the origin point in each of the sketches?

A: The cursor automatically snaps to the origin point, as well as other points on geometry within the sketch.

Step 2: Using the Loft Tool

The quickest way to create the bottle is by using the loft tool. "Lofting" comes from shipbuilding: it's the method shipbuilders use to connect the cross-sections of a ship structure to make the smooth form of the hull. It works basically the same way in 3D software- a new surface is created by connecting 2 or more cross-section profiles.

Create > Loft

Loft additional profiles, Operation: Join

Complete bottle form with Loft tool

To use this tool, I go to Create>Loft in the menu, click the profiles I want to use, and click OK. Fusion lets you select multiple profiles for single lofted objects which makes it really easy to create the object quickly. The bottle basically consists of 3 parts- the neck, the rim, and the cap.

Step 3: Create the Base Form

Now that I have my bottle as a starting point, I can design a bottle lock with the correct dimensions and features.

Construct > Offset Plane (5mm)

I start by offsetting a plane from the top of the bottle by 5mm. This seems like a reasonable thickness for the plastic shell that’s going to make up the clamp.

Sketch > Create Sketc (select plane)

Sketch > Project, Sketch > Offset (5mm)

I project the edge that represents the outside of the cap, then offset it by 5mm, staying consistent with my shell dimension. The clamp is going to have two mechanical parts- a hinge and a hasp (an opening for the padlock).

Sketch > Line

Sketch > Circle > 2-Point Circle

I start by drawing two lines to represent the vertical and horizontal centers of the circle. On the horizontal one, I create a 2-point circle with a 10mm Ø- this will be the hinge.

Q: How did I turn a Normal line into a Construction line in the video?

A: I select the line, right-click, then select "Normal / Construction" in the popup menu.

In Line tool, click and hold to create tangent line

Draw 4 tangent-tangent lines

I want to make a tangent line between the big circle and the 10mm circle I just made. To do this, all I have to do is select the Line tool, then click and hold on one of the circles. As I drag the mouse, the line stays tangent to the circle I clicked on. I click on the next circle at the tangent point, and I’ve got what I need. I repeat this step for the other three edges of the shape.

Construct > Offset Plane (5mm)

I want to stay consistent with my 5mm shell dimension everywhere, so I offset a plane from the underside of the ridge to use as the end of my clamp mass.

Create > Extrude (to plane)

I select the Extrude tool in the Create menu and click on the plane as the endpoint. Remember from the Stamp Lesson that the Extrude tool can create geometry in a few different ways. The default operation is "Cut", meaning the shape you've just extruded is going to excavate whatever other bodies it crosses. I’m going to need the bottle to remain intact for later, so I choose "New Component" under the "Operation" drop-down menu in the Extrude dialog box.

Step 4: Cut Out the Bottle Shape

Since my model is getting more complex, I’m going to start organizing it into components. Components make it much easier to visualize and edit your design when it has more than one part. When you create a component, you get a new item in the Browser that can be moved independently just by clicking and dragging.

You can also isolate Components and create sketches within them- this can make for a very organized project, especially when there's a lot of parts involved.

I select the bottle body from the browser, the Right-Click > Make Component from the pop-up menu.

Sketch > Create Sketch > Project

Sketch > Offset

The clamp is going to need a cutout that’s the same shape as the top of the bottle in order to work. To make sure everything fits together properly, I’ll need to give myself a little bit of wiggle-room on the cutout. To get this profile, I start with a center line based on the model origin, then create a sketch in the side work plane and project the profile lines of the bottle. I connect the dots where the profile tool doesn’t make lines to give myself the complete shape of the bottle’s side profile. Next, I use the Offset tool in the Sketch menu to give myself an offset I can work with.

Double-click dimension, change "1" to ".5"

1mm seems like too much of a gap, so I double-click the dimensions number and change it to .5mm.

Create > Revolve (operation: cut)

With my profile finished, I select the Revolve tool in the Create menu, select the two profiles I’ll need to create this cutout, and select my center line as the axis. The default operation is Cut, which is what I want.

To check the geometry, I change the Visual Style to Wireframe with Hidden Edges so I can see how close the features of the bottle are to the cutout in the clamp. To do this, I go to the toolbar at the bottom of the canvas, then Display Settings > Visual Style > Hidden Edges.

Now that I can see the insides of the model, moving the clamp from the side makes it pretty clear that it won’t be easy to pull the clamp up.

The clamp is going to work like a clam shell- a hinge on one end and a hasp on the other. To turn the mass into two parts, I go to the Split Body tool in the Modify menu. I select the lock component, then select the XY plane as the splitting tool. This gives me two separate parts that I can alter to create the hinge and hasp features.

Step 5: Create a Joint

Next, I want to edit the bodies to make the hinge feature. I need to see how the hinge action will work, so I’m going to create a joint between the two halves.

Joints can only be created between components, so since my lock now consists of two bodies in a single component, I select both bodies, Right-Click, and select Create Components from Bodies.

Browser > Component > Right-Click > Ground

I want one of the halves to stay in place when I test the motion of the joint, so I RightClick on the first half and select Ground.

Assemble > As-Built Joint

Select Center-Point of Circle

Preview Motion

Now that one of my halves is grounded, I go to the Assemble menu and click As-Built Joint, then select both halves of the lock. I change the Type from Rigid to Revolute, and the tool asks me to select a position. I click the center point of the arcs at the end of the components because this represents the center axis of the hinge in my design. The tool gives me a preview that looks good, so I click OK and try it out. All I have to do is click and drag the component to see how it moves.

{
    "id": "quiz-1",
    "question": "What happens when you move a joint if none of its components are grounded?",
    "answers": [
        {
            "title": "Nothing.",
            "correct": false
        },
        {
            "title": "All connected parts will move all over the place.",
            "correct": true
        },
        {
            "title": "Only the part you click-and-dragged will move.",
            "correct": false
        }
    ],
    "correctNotice": "You got it!",
    "incorrectNotice": "Nope! Without at least one grounded component, everything connected by a joint will move around."
}

Step 6: Create Hinge Features

Create Sketch on Top, Draw Circle

Create > Extrude (Join Operation)

With a preview of the motion, it’s easy for me to picture what I need to model. I go to Sketch > Create Sketch, click the top of one of the bodies of the lock component, then draw a Circle at the center point of the hinge's arc. I extrude this profile to the bottom of the part, then create another sketch on the bottom plane and draw another circle.

Select Top & Bottom

Mid-Plane Created

I create a Mid-Plane from the Construct menu to give me a horizontal plane I can use to split the hinge feature, then extrude the circle in the bottom profile to the mid-plane. This gives me the cutout in this part that will interlock with the other part.

Extrude Circle from Sketch, Select Mid-Plane

Step 7: Cut Out the Top

Now I need to create the opposite, interlocking feature on the half that’s been hidden in the last steps. All I have to do is create a sketch in the bottom plane, draw a circle, and extrude this profile to meet the other half. I create another sketch on the top and project the profile of the first half to give me the cutting profile that I extrude to finish the feature. My two halves now have clearance on their rotational axis.

Sketch Circle on Top, Extrude

Basic Form Complete!

I want the top of the lock to be open so you can see the logo on the bottle cap, so I create a circle on top of the lock and extrude it to cut through both halves.

Step 8: Recap

Now that we're completed the lesson, here's a quick recap of the skills we used to create the base model for the Bottle Lock.

Construction Planes

Construction planes are a constant companion in 3D modeling. In this lesson we used them to provide work planes to draw the circular profiles of the bottle, to mark the mid-plane of an object, and to split the clamp down the center line.

Loft Tool

The loft tool allows you to combine multiple profiles of different shapes and sizes into a single object. We used it to create the shape of our bottle because it was the quickest way to input the measurements we'd taken, but the tool can do a lot more than that. The example above could be a knob for a potentiometer or the base of a column.

Combining Bodies

The Combine command is important for creating complex forms. With it, we can join, cut, or intersect bodies to give us a new form. In the example above, I use the combine tool to cut the array of cylinders from the bigger body in the center. This gives me a straight profile with grooves along the outside surface.

Mechanical Joints
Joints give us the ability to make mechanical assemblies. In this lesson, we used them to help us design the form of the hinge before we even made that part, but joints can also be used with 3D models of manufactured parts like screws and bearings. Joint assemblies can be as simple as the hinge we made in this lesson or as complex as the interdependent parts of the telescope from this tutorial on Youtube. The contact sets function allows us to see the physical limits of our mechanical assemblies.

In the next lesson, we'll create the hinge pin feature, create clearances for movement, and refine the whole design so it's more ergonomic.