Part Modeling in Fusion
Learn how to create geometry based on sketches.
 
We'll be using a sketch of a mountain bike rocker arm to go through this lesson. At the end, you'll have it modeled like the example shown below.

Learning Objectives

  1. Creating geometry based on sketches
  2. Using sketch lines as reference
  3. Using sketches to drive changes in geometry

Dataset

In the Samples section of your Data Panel, browse to:

Basic Training > 04 - Modeling > 04_Model_from_sketch.f3d

Open the design and follow the steps below to complete the lesson.

Step-by-step Guides

Step 1: Select Profiles

Let's start with this sketch of the rocker arm. We're going to use this to create a solid body.

  1. Hold down Shift and select the profiles shown in the image.
  2. Make sure that the three center holes are the only profiles not selected.

Note: If you are having trouble selecting certain profiles, use your mouse wheel and zoom in closer; this should make selection easier.

Step 2: Start the Extrude command
  1. Right click on a selected area of the sketch and select Extrude.

     We're going to extrude the selected profiles.

 
Step 3: Define the extrude options in the Extrude dialog box
  1. Set Direction to Two Side.
  2. Set Extents to To.

You should now see two arrows appear on your selected sketch profiles. We're going to use these arrows to define where we want the extrusion to go. This is especially useful when you have set geometry you can use as reference, much like our sketch here.
 
Step 4: Set the distance for the left side
  1. Click once on the left arrow manipulator.
  2. Hover over the line sketch on the left side and click on the end point as the extent you want to extrude to.

Note: When Extrude extent is set to To, make sure you select the line sketch and not the rectangle sketch. When you've done this, the extrusion automatically terminates at that point. This selection is helpful when you have reference geometry you want to use to create new geometry.
 
Step 5: Set the distance for the right side
  1. Repeat Step 4 on the right side. Click once on the Right arrow manipulator.
  2. Hover over the line sketch on the right side and click on the end point as the extent you want to extrude to.
  3. Click OK (or press the Enter key) to finish the command.

Step 6: Turn sketch visibility back on
  1. Go to the browser and within the Sketches folder, click the light bulb icon next to Sketch1 to turn the visibility of that sketch back on.
Note: The visibility of a sketch is automatically turned off after a modeling action has been committed based on that specific sketch.
 
Step 7: Select a sketch profile behind an obstruction
  1. Select the circle profile to make an extrusion. If you find yourself in this situation where it is hard to select a specific geometry because it is being obstructed, then hover over the profile, click and hold. After a few seconds, you'll see a dialog menu show up, letting you choose what exact entity you'd like to select.
  2. Select Profile. You should now see the circle profile selected.

Step 8: Extrude the circle profile
  1. Right-click on the selected circle profile and select Extrude. We're going to choose this command again to create new geometry.

Step 9: Join the new extruded body
  1. Set the Direction to Symmetric. Leave Operation as Join.
  2. Drag the arrow to 20 mm.
Click OK to finish.
 
Step 10: Sketch a new circle profile
  1. Right click on Sketch1 in your browser and select Edit Sketch. This takes you back into the first sketch and creates more geometry. Notice that the timeline reflects us going back to this sketch item as well.
  2. Go to the Sketch drop-down menu and select Circle > Center Diameter Circle.
  3. Create a circle snapped the center with a diameter of 10 mm.

Click Enter twice to commit. Click Stop Sketch to exit sketch mode.
 
Step 11: Project the circle onto a new face
  1. Go to the Sketch drop-down menu and select Project / Include > Project.
  2. Select the outer face.
  3. Select the new circle sketch we just created.
Notice that the colour of the circle changes to purple which indicates it has been selected.
 
Click OK to finish, and Stop Sketch to exit the sketch mode.
 
You should now see that the circle is now projected onto the outer face of the model.
 
Step 12: Extrude the circle as a cut
  1. Select the projected circle profile, right-click and choose Extrude.
  2. In the command dialog, change the Extents to To.

Step 13: Make the cut
  1. Click on the Arrow Manipulator to activate the extrusion.
  2. Rotate the model to the other side so that we see the other face we want to extrude to. Click on that face and click OK to finish.
You should now see a cut made through the entire width of the model. This cut is now tied to the original circle sketch, thus allowing us to easily make dimension changes moving forward.
 
Step 14: Sketch a new circle profile
  1. We're going to move to the other side of the rocker model. Right click on Sketch1 in your browser and select Edit Sketch.
  2. Go to the Sketch drop-down menu and select Circle > Center Diameter Circle.
  3. Create a circle snapped the center with a diameter of 24 mm.
Click OK to finish, and Stop Sketch to exit the sketch mode.
 
Step 15: Repeat Project sketch workflow
  1. Go to the Sketch drop-down menu and select Project / Include > Project.
  2. Select the outer face.
  3. Select the new circle sketch we just created.
Click OK to finish, and Stop Sketch to exit the sketch mode.
 
You should now see that the circle is now projected onto the outer face of the model.
 
Step 16: Extrude the circle as a cut
  1. Select the area between the projected circle and the smaller circle, right-click and select Extrude.
  2. Drag the Arrow Manipulator to -10 mm. Click OK to finish.

Step 17: Mirror the cut on the other side

Now that we've made this cut, let's mirror it on the other side.

  1. Go to the Create drop-down menu and select Mirror.
  2. Go to timeline and select the last extrusion as the object we want to mirror.

Step 18: Mirror the cut on the other side

  1. Click the Mirror Plane option to activate which mirror plane to use.
  2. Select the origin plane that is in the middle of the model. Click OK to finish.
Note: If you are having trouble selecting the origin plane, remember to zoom out or click and hold to get the option to choose what you'd like to select.
 
Step 19: Use Press-Pull to cut
  1. Select the rectangle sketch at the bottom, right-click and use Press-Pull (on the right of your cursor).
  2. Drag the Arrow Manipulator through the model so the cut goes all the way through.
Notice that Press-Pull automatically became an Extrude command. This is the nature of Press-Pull: it adapts to the action when it gives you a predictable outcome. For example, if you had selected an edge and decided to use Press-Pull, it would have automatically created a Fillet.
 
Step 20: Add a couple of fillets
  1. finish the model by adding a couple of fillets on the inside edges. Select the inside edges by holding Shift.
  2. Right-click and select Fillet.

Step 21: Add a couple of fillets
  1. Drag the Arrow Manipulator to 5 mm. Click OK to finish.
 

Step 22: Making changes to your model

Since all the extrusions, mirror, and fillets are based on the original sketches, we can go back to Sketch1 and Sketch2 at any time and make dimension changes without needing to change each downstream feature or worry about any of them failing. You can also go to the Modify drop-down menu and select Change Parameters. This allows you to change any dimension in a chart form, assign custom names, set values or functions, and see the changes update instantly.

Step 23: Model complete!

Congratulations, you have completed this lesson on how to model based on sketches! You're ready to move on to the next lesson.
 
In the next lesson, we discuss how to Model based on a sculpted body.
 
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