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Assemble

Learn how to work with assemblies, assembly structure, joints and motion, and distributed design to create an assembly model using 2 approaches: traditional distributed design and top-down (multi-body).

Overview

Understanding assembly structure in Fusion 360 is important for establishing strong foundational knowledge.  These videos are a perfect way to start for anyone who’s new to Fusion 360.

  • Understand bodies and components

  • Assembly structure best practice

  • Reuse components as distributed parts

  • Understand joints

How to's

With a good understanding of bodies and components in Fusion 360, follow these how-to videos to learn about adding motion with joints, creating subassemblies, and working with a distributed design.

  • Choose the appropriate joint type

  • Choose the appropriate joint location

  • Manually add joint origins

  • Insert components & distributed design

Hands-on Exercises

Now you’re ready to put your skills into practice.  Follow these hands-on exercises to create bodies and components, work with distributed design and add motion with joints.

  • Creating new bodies and components

  • Inserting components used for distributed design

  • Manually adding joints

  • Working with subassemblies and as-built joints

  • Enabling Motion using Joints and Contact Sets

  • Updating designs using distributed components

Creating New Bodies and Components

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Goals:

  1. Understand when to create new components.
  2. Understand where geometry will be stored when it’s created.
  3. Practice duplicating 3D geometry in a design.
  4. Get comfortable moving bodies into components in the Browser.

Instructions:

  1. Download the file: http://app.solidprofessor.com/weblms/html5/f360/Hydraulic_Bottle_Jack.zip
  2. Upload it into Fusion.
  3. Create a new blank component in the design, and make sure it’s activated.
  4. Show the construction plane included in the design. Create a new sketch on this plane.

5. Create the sketch geometry as shown in the image. Make sure it’s fully defined, which requires creating sketch geometry from the intersections of the pins.

6. Extrude this sketch symmetrically, totallying to a width of 16 mm.
Note: You may have to hide some components from view.

7. Use the “Combine” command to create the holes in the new linkage component.

        a.  Select the bracket as the Target Body.

        b.  Select the two pins as the Tool Bodies.

        c.  Set the operation to “Cut”.

        d.  Make sure the “Keep Tools” option is selected.

8. Fillet the four corners along with the four edges at the angled section of the bracket using a radius of 5 mm.

9.   Activate the main assembly.

10. To add another instance of this linkage component, it will be mirrored in order to connect the same pins. To allow for the component to be mirrored, create a “Midplane” construction plane by referencing the end faces of the bottom pin.

11. Mirror the body about this plane.

12. Because the Mirror command created a new body and not a component, the bodies need to be separated out into two different components.

        a.  Create a new component at the top level of the assembly.

        b.  Drag the new body from the previous component into the new component.

        c.  Rename each component “Linkage – Left” and “Linkage – Right”.

Self-Check:

1. Click on one of the linkages in the design window, and then check which component is underlined in the Browser. Now click on the other linkage in the design window. Is a different component underlined in the Browser?

  • If so, good job!
  • It not, make sure that the two created components have a single body within each of them. If they don’t drag one body into the component that doesn’t have a body stored in it.

Inserting Components used for distributed design

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Goals:

  1. Understand how to insert one design into another design.
  2. Practice placing components using the “Move” command.
  3. Practice adding multiple instances of a distributed design.

Instructions:

  1. Download the files: http://app.solidprofessor.com/weblms/html5/f360/Inserting_Components.zip
  2. Upload the files into Fusion 360.
  3. Open the “2TonJack” design.
  4. Open the data panel, then right click on the “Caster” design and select “Insert into Current Design”.   

             a. Caster should be inserted in the correct location, so you can click “OK” in the “Move” dialog box.

5. Add another instance of the Caster into this design.

    a.  Can be inserted just like before, by right clicking on the design in the data panel and selecting “Insert into Current Design”.

    b.  Alternatively, it can be copied and pasted into the design.

            i.  Windows – Copy = Ctrl+C, Paste = Ctrl+V

            ii. Mac – Copy = Cmd+C, Paste = Cmd+V

6. Use the “Move” dialog box and the manipulator to move the new Caster over 158 mm and position it in the other hole of the Jack.

Self-Check:

  1. Select the “Measure” tool from the Inspect menu. Then measure the distance between the two cylindrical shafts protruding upward on the Casters. Is the maximum distance 168 mm?
  • If so, good job!
  • If not, make sure that both Casters are inserted in the design, and that the shafts on the Casters are centered within the holes on the Jack.

Manually Adding Joints

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Goals:

  1. Understand how to create an assembly from individual designs.
  2. Determine when a joint origin should be manually added at the assembly level or within the component.
  3. Understand which snap points to select on components in order to correctly create the joint.
  4. Practice adding different joint types to components.

Instructions:

  1. Download the file: http://app.solidprofessor.com/weblms/html5/f360/Manually_Adding_Joints.zip
  2. Upload each separate design into a single folder in Fusion 360’s data panel.
  3. Create a new design. Save this new design and name it “Clamp Joints”.
  4. Insert the component “Base” into the current design.

5. Ground the Base component.
6. Insert the component “Lever” into the design.

7.Add a Revolute joint between the center point of the cylindrical face on the Lever and the center point of the hole at the back of the Base.
Note: Be sure to “Flip” the orientation of the joint so that they match the components shown in the image to the right.

8. Open the “Lever” design.
9. Create a new joint origin centered between the two holes on the Lever.

10. Save the Lever design.
11. Switch back to the main assembly. To make sure the new joint origin is included in the assembly, right click on the Lever in the Browser and select “Get Latest”.
12. Add a Revolute joint between the center of the cylindrical face on the Connector and the newly created joint origin on the Lever.
Note: you may need to show the joint origin in the Browser.

13. Insert the component “Shaft” into the assembly.
14. Add a “Cylindrical” joint between the cylindrical face of the Shaft and the inner cylindrical face of the Base.
Note: Any point can be selected on these faces because of this joint type.

15. Use the Capture Position command so that the Shaft and Connector components don’t come into contact with one another.
Note: It may be advantageous to move the Shaft completely out of the Base so that the joint can easily be created afterward.

16. Add a Revolute joint between the center point of the hole at the end of the Shaft and the center point of the cylindrical face on the Connector.
Note: You may need to hide and show components in the Browser in order to select these points.

17. Insert the component “Clamp” into the design.
18. Create a Ball joint between the spherical face on the clamp and the spherical face on the Shaft.

19. Insert the component “Grip” into the design.
20. Create a Rigid joint between the Grip and the handle portion of the Lever.
Note: Be sure to select the center point of the curved edges on each component. Use the inner face of the Grip and the outer face of the Lever.
21. If needed, use the angle values in the Joint dialog box to adjust how the Grip lines up with the Lever.

Self-Check:

  1. Click and drag the Grip component. Is the Shaft sliding in and out of the Base? Is the Connector rotating as well as translating with the components?
  • If so, good job!
  • If not, make sure that there are six joints showing in the Browser, totaling to 3 Revolute joints, 1 Cylindrical joint, 1 Ball joint, and 1 Rigid joint. Also make sure that the Base is grounded.

Working with Subassemblies and As-Built Joints

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Goals:

  1. Practice creating components from bodies in order to create an assembly that enables motion.
  2. Understand how to organize components within subassemblies.
  3. Get comfortable creating As-Built Joints.
  4. Understand how to leverage copying and pasting components within an assembly.

Instructions:

  1. Download the file: http://app.solidprofessor.com/weblms/html5/f360/Piston_Linkage.zip
  2. Upload the .f3d file into Fusion 360.
  3. Create components from each body and rename them accordingly.
  • 2 “Arm” components
  • 1 “Piston – Inner” component
  • 1 “Piston – Outer” component

4. Create the Piston subassembly.

  • Create a new blank component within the main assembly.
  • Rename it “Piston Subassembly”.
  • Drag the two Piston components into this subassembly (the component icon will now switch to an assembly icon).

5. Add a Revolute as-built joint between the two arms.

  • Select both Arm components.
  • Change the joint type to “Revolute”.
  • Select the circular edge where both arms come into contact with one another.

6. Add a Cylindrical as-built joint between the two pistons.

  • Activate the Piston Subassembly.
  • Select both components.
  • Set the joint type to “Cylindrical”.
  • Select the center point on the face at the end of the component “Piston – Outer”, which is where the other Piston slides into it.

7. Reactivate the main assembly.
8. Create a Revolute as-built joint between the Piston Subassembly and the Arm at the bottom.

  • Select the bottom Arm component and the Piston – Inner component.
  • Change the joint type to “Revolute”.
  • Set the joint type to “Cylindrical”.
  • Select the center point of the inner cylindrical face on the Piston – Inner component.

9. Create a Revolute as-built joint between the Piston Subassembly and the Arm at the top.

  • Select the top Arm component and the Piston – Outer component.
  • Change the joint type to “Revolute”.
  • Select the center point of the inner cylindrical face on the Piston – Outer component.

10. Ground the lower Arm component.
11. Test out the motion of the assembly by clicking and dragging the top Arm component.

12. Click the “Revert” option in the Position menu.
13. Add another instance of the Piston Subassembly in the design.

  • Right click on the Piston Subassembly in the Browser and select “Copy”.
  • Press “Ctrl+V” on the keyboard (or “Cmd+V” for Mac users) to paste in the new instance of the subassembly.
  • Move the new subassembly 180 mm to the left so that the Pistons line up with the two Arms.

14. Add a Revolute as-built joint between the Piston Subassembly and the lower Arm component.
15. Add a Revolute as-built joint between the Piston Subassembly and the upper Arm component.

Self-Check:

  1. Are there 5 joints shown at the main assembly level in the Browser?
  • If so, good job!
  • If not, make sure that the cylindrical joints applied between the two pistons were added to the subassemblies.

2. Click and drag the top Arm component in the design window. Is it rotating while the Piston subassemblies slide in an out of one another?

  • If so, good job!
  • If not, make sure that one of the Arm components is grounded and that there are 7 total joints added in the assembly (two of which are found within the subassemblies).

Enabling Motion using Joints and Contact Sets

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Goals:

  1. Practice positioning components and enabling degrees of freedom by applying joints to components.
  2. Understand how to position components prior to creating a contact set.
  3. Get comfortable applying contact sets to the correct components in order to enable the proper mechanical motion.

Instructions:

  1. Download the file: http://app.solidprofessor.com/weblms/html5/f360/GenevaDrive.zip
  2. Upload into Fusion.
  3. Open the “GenevaDrive” design.
  4. The Rotor components need to be held together. Create a rigid group that contains all of these components.

5. Create a Revolute joint between the Rotor and the Frame.

    a. Select the center of the circular face where the spindle begins on the underside of the subassembly.

6. Make sure the blue cross piece is matching up with the circular face on the Rotor.

7. Move the rotor so that the white pin is located outside of the blue Cross piece.

8. Enable contact sets.

9. Create a new contact set between the blue Cross piece and the cylindrical face on the white pin.

10. Click and drag the Rotor in a circular motion to verify that the correct motion is produced in the assembly.

Self-Check:

  1. Does the blue Cross piece only spin when the white pin enters the slot?
  • If so, good job!
  • If not, make sure that the rigid groups were applied to the correct sets of components, and that the contact set was applied to the cross and the white pin.

Updating Designs using Distributed Components

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Goals:

  1. Understand how to make modifications to distributed components.
  2. Practice updating the larger assembly when a distributed component is modified.
  3. Get comfortable making modifications to components within a subassembly.

Instructions:

  1. Download the file: http://app.solidprofessor.com/weblms/html5/f360/2TonJack_and_Caster.zip
  2. Upload the files and open both.
  3. Bring up the “2 Ton Jack” design. Move down in the Browser and verify that the Casters are included as distributed designs.

4. Bring up the “Caster” design.

5. The Caster will be modified by creating a cutout on each tab on either side of the wheel. Isolate the component “Ork” to begin making the modification.

6. Show the sketch included in the design.

7. Create the cutout going through the part, as shown in the picture.

a. Select the center of the circular face where the spindle begins on the underside of the subassembly.

b. Set the Direction to “Two Side”.

c. Change the Extents to “All”.

d. Make sure the operation type is set to “Cut”.

8. Hide the sketch.

9. Unisolate the Ork component and save the design. Name the new version “Cutout Added”.

10. Switch back to the 2 Ton Jack design.

11. Update all versions of the Caster in the design by clicking the caution triangle at the top of the interface and then select “Get All Latest”.

Self-Check:

  1. Rotate the model and view each Caster subassembly within the 2 Ton Jack. Do both tabs on the Casters include cutouts?
  • If so, good job!
  • If not, make sure that the cutout was created in the separate Caster design. Also make sure that both instances of the Caster were updated to the latest version in the 2 Ton Jack assembly.