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Model

There are two ways to work in the Model environment, parametric and direct.  Learn about when, why and how to use parametric or direct modeling in Fusion 360.

Overview

It’s important to understand the differences between parametric and direct modeling.  With these videos you’ll get an overview of these two ways of modeling as we demonstrate Fusion 360 modeling best practices.

  • Parametric and direct modeling

  • Easily identify and modify model geometry

  • Use section analysis to view components or make measurements

How to's

Once you have a good understanding of parametric and direct modeling, learn how to create and work with 3D geometry using common features in Fusion 360.

  • Use Extrude to create 3D features

  • Use Revolve to create 3D geometry from profiles

  • Use Sweep to create a closed profile along a path

  • Use Loft to create geometry between points or profiles

Hands-on Exercises

Now you’re ready to put your skills into practice.  Try these hands-on exercises to get started.

  • Creating features from sketches

  • Adding features to a part

  • Modifying existing features

  • Working with draft, chamfer, combine and scale Commands

  • Working with Holes, Threads, and the Shell Command

  • Pattern and mirror commands

Creating Features from Sketches

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Goals:

  1. Successfully create a Sweep feature that incorporates guide rails.
  2. Extrude multiple sketch profiles using a single command.
  3. Create a Revolve feature as a new body.

Instructions: (sweep, two extrudes, revolve)

  1. Open the existing exercise zip file “Trumpet.zip”
    You can also open it here: Trumpet.zip.
  2. Upload the design in Fusion 360’s data panel.

3. Activate the Sweep command and create a Sweep feature to complete the body of the trumpet.

    a.  Set the Type to Path + Guide Rail and select the profile of the sweep feature. Be sure not to select the inner circular sketch profile, only the outer thin circular sketch profile.

    b.  Next, select the sketch connected to the center of the circle as the path. Be sure to select all of the sketch segments along this path.

    c.  Select the sketch connected to the outer edge of the circular profile as the guide rail. Continue selecting all sketch segments along this path as the total guide rail.

4. Extrude the trumpet keys 185 millimeters and set the operation to “Join” to combine this geometry with the previous sweep feature.

5.  Next, create the cut out of the shafts on the keys with an extruded cut at a distance of -20 millimeters.

6. Finally use a revolve feature to complete the mouthpiece.

        a.  Select the sketch as the profile.

        b.  For the axis select the sketch that acted as the path of the sweep.

        c.  Be sure to set the Operation to “New Body” so that this feature creates the mouthpiece as a separate body.

Self-Check:

  1. Set the material for the body by right clicking on the body in the Browser, and selecting
    “Physical Material.”
  2. Navigate to the “Metal” folder in the dialog box, and then drag “Brass” onto the main body, and “Silver” onto the mouthpiece body.
  3. To find the mass of the trumpet, right click on the component “Trumpet” at the top of the Browser and select “Properties”. What is the mass of the model?

        Did you get a value of 3873.579 grams? If so, great job.

        If not, make sure the following were done correctly:

  • “Brass” was set as the material for the body, and “Silver” was set as the material for the
    mouthpiece.
  • All of the correct paths and guide rails were selected to create the Sweep feature.
  • The extrusion depths were set to the correct values.
  • Check the document’s units.

Adding Features to a Part

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Goals:

  1. Create additional feature to existing bodies.
  2. Identify when to use a Loft feature in order to connect bodies that have different cross-sectional geometry.
  3. Control the shape of a loft feature by incorporating a guide type.
  4. Successfully create a Web feature to add strength to the model.
  5. Successfully create a Rib feature to add strength to the model.

Instructions: (Loft, Web, Rib)

  1. Open the existing exercise zip file “Gas_Pedal.zip”
    You can download  it here: Gas_Pedal.zip
  2. Upload the design in Fusion 360’s data panel.

3. Expand the Sketches folder in the Browser and turn on the “Loft Centerline” sketch.

4. Activate the Loft command to create the connection between the pedal and the base.

    a.  Select the Face on the base in the shape of an “I” that protrudes out towards the pedal.

        b.  Select the split face on the back side of the pedal facing the base.

    c.  Under the Guide Type in the dialog box, activate the “Centerline” option and select the “Loft Centerline” sketch in the canvas.

    d.  Click OK to complete the command.

5. Turn on the “Web” sketch.

6. Activate the Web command to create the reinforcing geometry within the loft feature.

    a.  Select the 11 sketch lines that intersect with the loft.

    b.  Set the Thickness to 2 mm, along with the other parameters shown in the dialog box to the right.

    c.  Click OK to complete the command.

7. Turn on the “Rib” sketch.

8. Activate the Rib command to create the Rib and finish model.

    a.  Select the angled sketch line as the Curve.

 

Activate the Rib command to create the Rib and finish model.8

    b.  Set the Thickness Option to “Symmetric”.

    c.  Set the Depth Option to “To Next”.

    d.  Set the Thickness to 7.5 millimeters.

    e.  Click OK to complete the command.

 

Self-Check :

  1. Set the material for the model by right clicking on the component “Gas_Pedal” in the
    Browser, and selecting “Physical Material”.
  2. Navigate to the “Plastic” folder in the dialog box, and drag “ABS Plastic” onto the body in the canvas.
  3. To find the mass of the body, right click on the component “Gas_Pedal” at the top of the Browser and select “Properties”. What is the mass of the model?

        Did you get a value of 262.074 grams? If so, great job!

        If not, make sure the following were done correctly:

  • “ABS Plastic” was set as the material.
  • Make sure the “Loft Centerline” has been selected as centerline for the Loft feature.
  • Make sure all 11 sketch lines are selected in the Web feature.
  • Make sure the Web and Rib features are set to the correct depths.
  • Check the document’s units.

Modifying Existing Features

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Goals:

  1. Edit existing features to make changes that align with the model’s design intent.
  2. Identify when to edit a feature in order to correctly modify the geometry.
  3. Identify when to edit a sketch profile in order to correctly modify the geometry.

Instructions:

  1. Open the existing exercise zip file “Canoe.zip”
    You can also open it here: Canoe.zip.
  2. Upload the design in Fusion 360’s data panel.

3. To create a curved contour at the ends of the canoe, edit the Sweep feature by double clicking it in the timeline.

    a.  Change the type to Path + Guide Rail and select the Shape sketch in the canvas as
the guide rail.

4.  Next, edit the Loft feature to refine the shape of the underside of the canoe.

    a.  Edit Profile 2 and change the profile type to be Point Tangent

    b.  Set the Tangency Weight to 1.

        c.  Click OK to complete the command.

5. Expand the Sketches folder in the Browser and edit the sketch “Seats”.

6. Dimension one of the sketch lines from the center of the canoe a distance of 45 millimeters. Once the dimension is set close the sketch.

Self-Check:

  1. Set the material for the model by right clicking on the component “Canoe” in the Browser, and selecting “Physical Material”.
  2. Navigate to the “Wood” folder in the dialog box, and drag “Cherry” onto the body in the canvas.
  3. To find the mass of the body, right click on the component “Canoe” at the top of the Browser and select “Properties”. What is the mass of the model?

        Did you get a value of 6.695 grams? If so, great job.

        If not, make sure the following were done correctly:

  • Double check that “Cherry” was set as the material.
  • Make sure the Sweep feature’s type is set to Path + Guide Rail and has the sketch
    selected as the guide rail.
  • Go back and check that the Loft feature’s second profile is set to Point Tangent and has a Tangency Weight set to 1.
  • Make sure the seats are dimensioned 45 millimeters from the center of the canoe.
  • Check the document’s units.

Working with Draft, Chamfer, Combine, and Scale Commands

x/x  

 

Goals:

  1. Use the draft command to quickly set an entire face at an angle.
  2. Apply a chamfer in order break a sharp edge.
  3. Use the combine tool to join multiple bodies into one body.
  4. Shrink an entire body using the Scale command.

Instructions (Extrude, Loft, Chamfer, Combine, Shell, Web, Scale) :

  1. Open the existing exercise zip file “Door_Stop.zip”
    You can also open it here: Door_Stop.zip.
  2. Upload the design in Fusion 360’s data panel.

3. To begin, launch the Extrude command and extrude the semicircular sketch profile upward 50 millimeters.

4.  Extrude a new body of the longer portion of the of the Base Sketch profile by 50 millimeters.

5. Enable the Draft command to create the angled face of the second extruded body.

    a.  Expand the Bodies folder in the Browser and hide the first extrude.

    b.  Select the back face of the model that comes into contact of the hidden extrude as the draft plane.

    c.  Select the top face of the model as the face to draft.

 

    d.  Use a 10 degree angle for the draft and make sure the draft is in the correct direction, making sure the face tapers downward.

 

    e.  Click “OK” to finish the command.

6. Expand the bodies folder in the Browser and unhide the first extrude.

7. Activate the Draft command again to angle the outer faces of the model.

    a.  Select the sketch profile on the bottom face of the model as the plane.  

    b.   Hold down the Ctrl key (or Command for Mac users) and select the three larger side faces of the model and set the draft angle to 15 degrees. Make sure the draft is going in the correct direction. 

    c.  Click “OK” to finish the command.

8. Apply a chamfer to the shortest edge of the top angled face.

    a.  Set the Chamfer Type to Distance and Angle

    b.  Select the short edge.

    c.  Set the distance to 10 millimeters and the angle to 35 degrees.

    d.  Click “OK” to complete the command. 

9.  Next, use the Combine command to join the two bodies of the model.

    a.  Select the first extrude of the model as the Target Body and the second extrude as the Tool Body.

    b.  Make sure the operation is set to “Join”.

    c.  Click “OK” to complete the command.

 

10. Expand the Sketches folder and turn off the “Base Sketch”.

11. Apply an Inside shell with a thickness of 5 millimeters to the bottom face of the model.  

 

 

12. Expand the Sketches folder in the Browser and turn on the “Web Sketch”.

13. Enable the Web command to create the support material underneath the model.

    a.  Select the four sketched lines as the curves.

    b.  Set the Thickness Options to Symmetric, the Depth options to To Next, and the Thickness 5 millimeters.

    c.  Make sure the Web is being created in the correct direction. 

    d.  Click “OK” to finish the command.

14. Turn off the “Web Sketch” and turn on the “Base Sketch” once again.

15. Use the Scale command and expand the model by 5%.

    a.  First choose the point to scale about. Select the point on the “Base Sketch” where the construction line intersects the semi-circular profile.

 

    b.  Set the Thickness Options to Symmetric, the Depth options to To Next, and the Thickness 5 millimeters.

    c.  Keep the Scale Type at Uniform and set the scale factor to 1.05.

    d.  Click “OK” to finish the command.

Self-Check:

1. Mass Check:

    a.  Set the material for the model by right clicking on the component “Door Stop” in the Browser, and selecting “Physical Material”.

    b.  Navigate to the “Plastic” folder in the dialog box, and drag “Rubber” onto the body in the canvas.

    c.  To find the mass of the body, right click on the component “Door Stop” at the top of the Browser and select “Properties”. What is the mass of the model?

Is the Mass of the part 214.7 grams? If so, good job!

If not make sure the following steps were executed correctly:

  • Each Extrusion was set to the correct depth.
  • Each Draft was set to the correct angles.
  • The Shell and Web features were set to the correct thickness.
  • The Scale feature has expanded the model by 5%.

2. Number of Bodies:

Expand the Bodies folder in the Browser and check how many bodies are present. Is there only one body? If so, good job!

If not, make sure the following was done correctly:

  • The Combine feature has an operation set to join.

 

Working with Holes, Threads, and the Shell Command

x/x  

 

Goals:

  1. Use the hole command instead of an extruded cut
    to create specific hole types.
  2. Apply a shell to hollow out bodies of a model.
  3. Apply threading to a shaft using a Thread command.

Instructions (Holes, Threads, Shell):

  1. Open the existing exercise zip file “Threaded_Mount.zip”
    You can also open it here: Threaded_Mount.zip.
  2. Upload the design in Fusion 360’s data panel.

3. Expand the Sketches folder and turn on “Hole Feature” sketch.

4. Enable the Hole command to create the four counterbore holes.

    a.  Select the four points on the corner of “Hole Feature”.

    b.  Set the Hole Type to “Counterbore”, the Diameter to 7.5 millimeters, the Tip Angle to 118 degrees, the Counterbore Depth to 2.5 millimeters, the Counterbore Diameter to 10 millimeters, and the Extents to “All”.

    c.  Make sure the Hole command is going in the correct direction.

    d.  Click “OK” to complete the command.

5. Enable the Shell command to hollow out the underside of the model.

    a.  Select the back flat face of the mount as the face to shell.

    b.  Set the Inside Thickness to 2.5 millimeters and the Direction to “Inside”.

    c.  Click “OK” to complete the command.

6. Drag the marker to the end of the timeline to include all of the features in the model.  

7. Turn on the sketch “Web Feature”.

8. Enable the Web command to create the supports on the inside of the model.

    a. Select the four sketch lines as the curves. Set the Thickness Options to “Symmetric”, the Depth Options to “To Next”, and the Thickness to 2.5 millimeters.

    b.  Click “OK” to complete the command.

9. Apply a chamfer to the end of the shaft protruding through the model.

    a.  Select the circular edge on the end of the cylindrical protrusion.

    b.  Set the chamfer type to “Equal Distance” with a distance of 3 millimeters.

10. Use the Thread command to create the threading on the shaft.

    a.  Activate the Thread command and select the outer face of the shaft as the face to which the thread is applied.

    b.  Check the “Modeled” and “Full Length” boxes to have the threads become modeled geometry that extend along the shaft up to the chamfered face.

    c.  Set the Threaded Type to “ISO Metric profile”, the “Size” to “39.0 mm”, the “Designation” to “M39x4”, the “Class” to “6g”, and the “Direction” to “Right hand”

    d.  Click “OK” to complete the command.

Self-Check:

  1. Set the material for the body by right clicking on the model name “Threaded Mount” at
    the top of the Browser, and selecting “Physical Material”.
  2. Navigate to the “Metal” folder in the dialog box, and then drag “Steel, Alloy” onto the body in the canvas.
  3. To find the mass of the body, right click on the component “Threaded Mount” at the top of the Browser and select “Properties”. What is the mass of the model?

        Did you get a value of 1462 grams? If so, great job.

        If not, make sure the following were done correctly:

  • Make sure the diameter and depth of the counterbore holes are set to their appropriate
    values.
  • Make sure the shell is set to the proper thickness.
  • Check that the Web feature and has the correct thickness.
  • Make sure all of the Thread properties are correctly defined.

Pattern and Mirror Commands

x/x  

 

Goals:

  1. Recognize when to use specific pattern features.
  2. Successfully apply path and circular pattern features.
  3. Use the mirror tool to simplify the creation of geometry.

Instructions: (sweep, two extrudes, revolve)

  1. Open the existing exercise zip file “Turbine.zip”
    You can also open it here: Turbine.zip.
  2. Upload the design in Fusion 360’s data panel.

3. Activate the “Pattern on Path” command.

    a.  Set the Pattern Type to “Pattern Features”.

    b.  Select the extruded cut of the turbine blade on the timeline as the objects.

    c.  Select the outside longitudinal edge of the blade as the path.

    d.  Enter a Distance of “80 millimeters” and with a Quantity of “10”.

    e.  Click “OK” to complete the command.

4. Next, activate the “Circular Pattern” command.

    a.  Set the Pattern Type to “Pattern Bodies”.

    b.  Select the turbine blade as the object and the circular edge at the base of the turbine as the axis.

    c.  Set the Type to “Full” and the Quantity to “15”.

    d.  Click “OK” to complete the command.

5. Finally, Mirror the features about the bottom flat face of the turbine base.

    a.  Enable the “Mirror” command.

    b.  Set the Pattern Type to “Pattern Bodies”.

    c.  Select the base and all 15 turbine blades as the Objects.

 

    d.  Select the bottom flat face of the base as the Mirror Plane.

    e.  Click “OK” to complete the command. 

Self-Check:

  1. Set the material for the body by right clicking on the component in the Browser, and selecting “Physical Material”.
  2. Navigate to the “Metal” folder in the dialog box, and then drag “Aluminum” onto the component in the canvas.
  3. To find the mass of the model, right click on the component “Turbine” at the top of the Browser and select “Properties”. What is the mass of the model?

        Did you get a value of 4293.7 grams? If so, great job.

        If not, make sure the following were done correctly:

  • For the “Pattern on Path” pattern feature, check the distance was set correctly.
  • Make sure that both pattern features have the correct number of instances.
  • Assure all the bodies have been selected for the mirror feature.