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Sketch

Learn to create 3 dimensional features from sketches.  

Overview

To get started, get an overview of sketch elements, learn the importance of design intent to create predictable results, and understand the importance of fully defining sketch entities.

  • Sketch philosophy and considerations

  • Working with the sketch grid

  • Design intent strategy

How to's

Once you understand the foundation for sketching in Fusion 360, follow these videos to explore on your own.

  • Start a new sketch

  • Edit a sketch

  • Fully define sketch entities with dimensions and constraints

  • Use splines for fluid or organic curves

Hands-on Exercises

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

  • Sketching basics

  • Intermediate sketching

  • Modifying sketches 1

  • Modifying sketches 2

  • Adding constraints and dimensions

  • Fully-defining a sketch

Sketching Basics

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Goals:

  1. Getting comfortable switching between
    sketch tools.
  2. Choosing the correct sketch tool to use to recreate a sketch profile.
  3. Practice selecting key points in the sketch associated with the different sketch commands.

Instructions:

  1. Open a new Fusion 360 document.
  2. Create a Sketch on any of the default planes.
  3. Use one of the Rectangle commands to create the main handle of the tuning fork. Be sure it’s positioned correctly.

4. To finish sketching the handle, add a circle at
the bottom.

Note: Notice where the circle intersects the rectangle, along with the constraints added. Be sure to select a circle command that will help you easily create this sketch entity.

5. Begin creating the upper part of the fork by drawing the three lines in a chain on the left. Make sure the second line is vertical, which is confirmed by the vertical glyph appearing next to the line. The third line should be at a right angle to the second, indicated by a perpendicular glyph appearing in the corner.

6. Sketch the inside of the fork, made up of two lines and an arc.

    Note: this section can be sketched using only the line tool.

7. Finish the sketch by recreating the geometry from the left side on the right side.

Self-Check:

  1. Does the rectangle handle in the sketch have construction lines and is it centered on the origin? 
  • If so, good job! 
  • If not, double check which rectangle command was used to create this sketch entity. Another one may need to be used instead.

Self-Check:

2. If you move the bottom right point on the rectangle, do the rectangle and circle change in size simultaneously? Do the angled lines also change in size?

  • If so, good job!
  • If not, double check that a coincident constraint was added when the circle was drawn. Also make sure that the entire profile is enclosed (highlights on screen) and that all of the lines connect.

Intermediate Sketching

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Goals:

  1.  Determining the order that sketch entities are created.
  2. Getting comfortable using different sketch tools.
  3. Practice selecting key points in the sketch associated with the different sketch commands.

Instructions:

  1. Open a new Fusion 360 document.
  2. Create a sketch on one of the default sketch planes.
  3. Create the two sketch entities shown to the right. Be sure to decide which sketch entity should be drawn first, and to utilize the origin when sketching the first sketch entity.

4. Connect the two sketch entities on the left
side with a single line.

5. To complete the body of the iron, add two lines and an arc. Make sure that a parallel constraint is added between the horizontal line and the top of the rectangle.  

6. Add a six point spline to the sketch as the handle of the iron.

Note: Be sure to move the key points and handles to approximate the same shape shown in the image to the right.

7. Finish the sketch by adding a smaller inner circle that shares the same center point as
the other circle.

Self-Check:

  1. Move the top right corner of the body down and to the left. Does the outer circle become larger and does the shape of the spline change?  
  • If so, good job! 
  • If not, double check that the top line of the body is parallel to the top of the rectangle. Also check that the arc and this same line have a tangent constraint added. 

Modifying Sketches 1

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Goals:

  1. How to make modeling more efficient.
  2. Practice using construction geometry.
  3. Recognizing symmetry in a sketch.

Instructions:

  1. Open a new Fusion 360 document.
  2. Create a Sketch on any of the default planes.
  3. Add a rectangle to the sketch, keeping in mind how it relates to the origin.

4. Create a spline that will be the top of the scissors.

Note: Note the start and end points of the spline.

5. Trim away geometry to make the sketch resemble the image to the right.

6. Add an angled construction line to the sketch.

7. Mirror the top blade across the construction line to create the second blade.  

Self-Check:

  1. Drag the straight edge of the bottom blade upward. Does the angle between the scissor blades decrease?
  • If so, good job! 
  • If not, double check that the endpoint of the construction line is connected to the bottom right corner of the upper scissor blade.

Modifying Sketches 2

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Goals:

  1. Practice creating sketch entities from existing 3D geometry.
  2. How to create sketch entities when existing 3D geometry blocks the view of the sketch.
  3. Understanding how a single sketch can be used to create multiple 3D features.

Instructions:

  1. Open the existing exercise file
    “Banana_Hook.igs” You can download it here: http://app.solidprofessor.com/weblms/html5/f360/Banana_Hook.zip
  2. Create a sketch on the bottom face of the body.
  3. Switch to the “Top” view.
  4. Project the outer edges of the part onto the sketch plane, as seen in the image to the right.

5. Draw a line to close off the projected sketch profile.

Note: enabling the Slice option from the Sketch Palette can help when working on this sketch.

6. In order to add sketch fillets on the corners, the link to the projected geometry needs to be broken. Break the link to projected geometry for the two short horizontal segments on the left.  

7. Add 10 mm sketch fillets to the two corners on the left side of the sketch.

8. Draw a 10 mm circle at the center point of the arc in the upper left corner. Be sure to enter the diameter value into the entry box.

9. Use the Rectangular Pattern command to create additional circles in two directions. Set the horizontal spacing to 145 mm and the vertical spacing to 40 mm.

10. Create the baseplate by creating an “Extrude” feature. To do this, go to the “Create” pull-down menu and select “Extrude”. Then select all of the enclosed profiles in the sketch (total of six). Make sure the arrow is pointing downward, which can be dragged in the correct direction. Set the “distance” in the dialog box to 5 mm, along with the “Operation” type to “New Body”. Click OK.

11. Create the four feet of the baseplate using the Extrude command once again. Go to the
“Sketches” folder in the Browser, and make sure the most recent sketch is active with the light bulb icon on. Activate the Extrude command. Select the 4 circular sketch profiles. Set the distance to 10 mm. Then set the Operation type to “Join” and click OK.  

 

Self-Check:

1. Find the volume of the part by expanding the “Bodies” folder in the Browser, then right clicking on the body and selecting “Properties”. Is the volume of the
body 9.713E+05 mm^3?

  • If so, good job!
  • If not, be sure to check the following:
    1. The fillet radii are 10 mm and the circle diameter is 10 mm.
    2. The first Extrude’s depth is 5 mm and includes all six profiles.
    3. The second Extrude’s depth is 10 mm and includes all four circular profiles.

Adding Constraints and Dimensions

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Goals:

  1. Understand the workflow of adding constraints.
  2. Get comfortable applying a variety of constraints to relate sketch profiles.
  3. Reinforce the best practice of adding constraints before sketch entities are dimensioned.
  4. Practice adding dimensions to the correct sketch entities.

Instructions:

  1.  Open the existing exercise file
    "Pocket_Knife.f3d". You can download it here: http://app.solidprofessor.com/weblms/html5/f360/Pocket_Knife.zip
  2. Edit the sketch.

3.  Add constraints to the body of the pocket knife:  

  • Tangent constraint - between the top of the rectangle and the arc on the right.
  • Midpoint constraint - between the center point of the arc on the left and the left side of the rectangle.

4. Add two dimensions to the body of the pocket knife:  

  • Dimension either arc to have a radius of 3 mm.
  • Dimension one side of the rectangle to have a length of 60 mm.

5. Add three constraints to the scissor blade profile:

  • Symmetric constraint - the two inner flat edges of the scissor blades.
  • Equal constraint - the bottom of the scissor blade profile and the left side of the rectangular body.
  • Coincident constraint - the center points of these same two arcs.

6. Reposition the scissor blade profile and add a dimension:

  • Drag the tip of the left blade to move the scissors closer to the pocket knife body.
  • Dimension one of the arcs at the end of the scissors to have a 7 mm radius.

7. Add two constraints to the bottle opener profile:

  • Perpendicular constraint - the bottom edge on the left and the straight line connected to it on the right.
  • Perpendicular constraint - the top line inside the gap and the line connected to it on the left.

8. Add three more constraints to the bottle
opener profile:  

  • Colinear constraint - the two lines on the bottom of the bottle opener.
  • Concentric constraint - the arc at the end of the bottle opener and the arc on the right side of the pocket knife body (rectangular profile).
  • Equal constraint - the same two arcs.

Self-Check:

1. Are all three profiles (the body of the pocket knife, the scissors, and the bottle opener) connected together with arcs of the same radii?

  • If so, good job!
  • If not, double check that the coincident and concentric constraints added to connect them together were the last constraints applied to
    each profile. (Can use the “Undo” and “Redo” buttons at the top to
    check the order).

Self-Check:

2. Are the scissors and the bottle opener able to move inward toward the body
of the pocket knife?

  • If so, good job!
  • If not, double check that all three constraints were added to the scissors and that all five constraints were added to the bottle opener. (Can use the “Undo” and “Redo” buttons at the top to check the order.)

Fully-Defining a Sketch

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Goals:

  1. Practice applying the correct constraints and dimensions to sketch entities.
  2. Understand when to use constraints vs. dimensions to fully define a sketch.
  3. Determine how under-defined sketch entities can be made fully-defined.

Instructions:

  1. Open a new Fusion 360 document.
  2. Create a Sketch on any of the default planes.
  3. To begin sketching the geometry for a wall outlet cover, sketch a 2-point rectangle. Be sure that the origin is positioned inside of the rectangle.
  4. Create a construction line between the midpoints of the rectangle’s sides.

5. Add a circle with its center point located at the midpoint of the construction line.

6. Sketch a rectangle above it to begin creating the outlet’s cutout.

7. Sketch two arcs on the left and right sides of the rectangle.

8. Change the left and right sides of the rectangle to construction lines.

9. Mirror the cutout to the lower half of the outlet cover.

10. With the general shape in place, it’s time to add constraints. Add a concentric constraint to the two arcs on the top outlet cutout.

11. Add a vertical constraint to the center point of these arcs and the center point of the smaller circle at the center.

12. Add an equal constraint between the two arcs of the cutout.

13. Add a coincident constraint with the origin and the center point of the smaller circle.  

14. Add dimensions to the outer rectangle. The width is 70 mm and the height is 114 mm, as shown in the image to the right.

15. Dimension the screw hole at the center to have a diameter of 12 mm.

16. Position the bottom edge of the cutout on top 25 mm above the horizontal
construction line.

17. Dimension the cutout to have a height of 28 mm.

18. Dimension one of the arcs on the top cutout to have a radius of 17 mm.  

Self-Check:

1. Is the sketch fully-defined, with all sketch entities shown in black?

  • If so, good job!
  • If not, drag any under-defined sketch entities in the canvas to see how they are unconstrained. Then check if a constraint or dimension wasn't added to this sketch entity