TekZone Robotics: Introduction to Robotics

  • Prep Work
  • Introduction to Robotics
  • Sensors
  • Motors
  • Computer-Aided-Design
    • Fusion 360 – using “sketch” tools
      45 min
  • Project: Rover Robot Design
  • Project & Time Manager
  • Kinematics
  • PID Control
  • Computer Vision
  • Robotics Arm Design
  • Project: Putting all Together
  • Impact Project: Assess
  • Impact Project: Design
  • Impact Project: Implementation & Test
  • Impact Project: Finalize
  • Impact Project: Showcase

Fusion 360 – using “sketch” tools

Objectives

  • Identify use cases for Sketch tools.
  • Use Browser and Timeline to identify and edit sketches associated with features..
  • Edit sketches associated with features after they have been created.

Materials

Laptop with Fusion 360 installed

Instructions

1- Open the “TekZone Exercises” project if not open already. Skip to Step 2 if the project is still open from Lesson 3.
Click Show Data Panel, click the left arrow to Leave Data Details, and double click TekZone Exercises to open the course project.

2- Verify that the component “Lesson 3 Box” is in the project. In this lesson, we will create a similar component using explicit Sketch tools.

3- Click File > New Design if not already in a new design. Click Save to save the new component to the project. Name the component “Lesson 4 Box”. This saves it to the project on the cloud, not to a local location on your computer.

4- Verify that the name of the part (Lesson 4 Box) is displayed 1) in the tab at the top 2) in the browser and 3) in the Data Panel on the left side of the window. The version indicator (in this picture v1) increments every time the part is saved.

5- Close the Data Panel by clicking the X in the upper right corner of the panel or clicking Hide Data Panel.

6- We want to start the component by creating a box similar to in Lesson 3. To do this, we will need a sketch in the XZ-plane that will be extended along the Y-axis to create a solid volume. Select the Create Sketch tool in order to start a sketch. You can do this a few ways.

  • Click the Create Sketch tool shortcut in the Toolbar.
  • Click Sketch to open the Sketch palette and click the Create Sketch
  • Press S on the keyboard to open the Model Toolbox and search for the Create Sketch tool. Press Enter or click Create Sketch to select the tool.

 

7- Similarly to in Lesson 3, select the XZ-plane to begin creating our component. This will assign the sketch to the XZ-plane and allow us to create 2D drawings on the plane.
Note: The color axes correspond with the axes in the ViewCube at the top right corner of the workspace. Y-axis is green, Z-axis is blue, and X-axis is red. Select the XZ-plane that share the blue and red axes.

8- This will reorient the window so we are looking perpendicular on the XZ-plane.

9- We want to create a square to be the base of our box. Click Sketch and the move your mouse over the Rectangle submenu to show the three ways we can create a rectangle.

  • 2-Point Rectangle will specify the two opposite corners of the rectangle. The sides will automatically be either Horizontal or Vertical. This rectangle type is good for most cases that need Horizontal and Vertical sides.
  • 3-Point Rectangle will specify 3 points of a rectangle and use geometry to add the 4th point. The sides will NOT automatically be Horizontal or Vertical. This rectangle type is good for shapes that should not be Horizontal or Vertical.
  • Center Rectangle will specify the center of the rectangle and a corner, geometry and trigonometry relationships will add the other 3 points. This rectangle type is good when the rectangle needs to be centered on a point.

10- For this sketch, we want the rectangle to be centered at the Origin. Click Center Rectangle.

11- Click on the Origin first to specify the center of the rectangle. Click again to specify the corner of the rectangle. You can also type in “40 mm” to specify the initial dimensions.

12- Press Esc on your keyboard to deselect the Center Rectangle tool.

13- Notice the rectangle has a blue border. This means the sketch is Unconstrained. You can click and drag on any of the corners to change the size of the rectangle. The goal of each sketch is to be Constrained using both Dimensions and Geometric Constraints. This locks sketches in place and allows for more consistent modeling.

  • Dimensions assign numeric values (either explicit or based on other values in the model) to parts of the sketch.
  • Geometric Constraints assign relationships between different parts of your sketch. Examples include Horizontal, Vertical, Parallel, Perpendicular, Equal, Coincident, Tangent, etc.

14- Notice the Center Rectangle we created already has some Geometric Constraints.

  • The midpoint of the diagonal construction lines is Coincident with the Origin.
  • The opposite sides of the rectangle are Parallel to each other.
  • The top and left sides of the rectangle are Perpendicular to each other. This ensures that the rectangle keeps right angles.
  • The top side of the rectangle is constrained Horizontal/Vertical. Because the other sides are all Parallel or Perpendicular to the top side, this locks all of the sides either horizontal or vertical.
  • The endpoints of the diagonal construction lines are Coincident with the corners of the rectangle.

All of the contraints above ensure that the rectangle is centered at the origin and the sides are all parallel or perpendicular to each other as well as horizontal and vertical. We will need to add constraints to specify the lengths of the rectangle sides.

15- Select the Sketch Dimension You can select the tool by clicking Sketch and the clicking Sketch Dimension or by using the keyboard shortcut D when in the workspace.

16- With the Sketch Dimension tool active, click the top side of the rectangle. Click again in the blank space above the rectangle to place the dimension. Alternatively, you can also click the left side of the rectangle, then the right side of the rectangle to dimension the distance between the two sides (which is the same as the length of the top side). Because of our geometric constraints, both methods will have the same result.

17- Click again to select the location for the dimension. Enter 40 mm for the length of the dimension.

18- Notice this changes in color of the left and right sides of the rectangle from blue to black. This means that the sides are Constrained meaning they will not move in the sketch. Try to click and drag the left and right edges to move the sides. They should not move because they are properly Constrained.

19- Click and drag the bottom side of the model down. The line moves because it is Unconstrained. Notice the top side of the model moves up. This is because we have the rectangle centered on the Origin.

20- We need to set a constraint for the length of the left and right sides of the rectangle. We can dimension this to 40 mm. However this makes it more difficult to change the model later because we will need to change both dimensions to keep the rectangle a square. We can use Geometric Constraints to set the sides equal to each other.

21- Click the top edge of the rectangle. Notice the Sketch Palette appears.

22- Hold Shift and click on the left side of the rectangle. Click on Constraints in the Sketch Palette to show all available constraints between the two lines.

23- Click Equal to set the the top and left sides equal. Because of other geometric constraints, the right and bottom sides are equal as well without needing their own Equal constraint between them.

24- Notice the lines in the sketch changes and are all black. This means that the entire sketch is Constrained and can be consistently used in features in the model.

25- The sketch is now ready to be used in other parts of the model. Click Stop Sketch to exit the sketch.

26- Next we want to use the sketch to create a physical object in our model. Select the Extrude Similar to Create Sketch, there are multiple ways to select the tool.

27- Select the Extrude tool in order to create solids from sketches. You can do this a few ways.

  • Click the Extrude tool shortcut in the Toolbar.
  • Press E on the keyboard.
  • Click Create to open the Create palette and click the Extrude
  • Press S on the keyboard to open the Model Toolbox and search for the Extrude tool. Press Enter or click Extrude to select the tool.

28- With the Extrude tool active, select the area inside the rectangle by clicking inside the rectangle.

29- To create a solid similar to the Box from Lesson 3, we want the height of the box to be 40 mm. Set the Extrude Distance to 40 mm. Click OK to submit changes and create the solid.

30- Click Home on the ViewCube to reset your view to the original home view. Zoom out to see the whole solid.

 

31- Notice in the timeline it took two tools to create the box instead of one. 1) A sketch to define the geometry in a plane and 2) another tool to create a solid by extending the plane in another dimension.

32- Also notice the browser has headings for Bodies as well as Sketches. This is different than in Lesson 3 where we modeled the entire component without sketches.

33- To create a cavity similar to the Shell tool, we will need to create a sketch on the top face of the extruded box.

34- Select Create Sketch and click on the top face of the cube to set the sketch plane. Sketches can be created on any flat surface including Model Planes, Faces, Reference Planes, etc.

35- This will reorient the window so we are looking perpendicular on the top face of the box.

36- We want our sketch to imitate the Shell tool, so we need to create a sketch that is offset from the outside edge of the box by 5 mm. The sketch should be created so that it can update depending on if the dimensions of the box change. We will use the Offset tool to create a sketch that is offset from other features by a certain distance.

37- Select the Offset You can do this a few ways.

  • Click Sketch to open the Sketch palette and click the Offset
  • Press O on the keyboard.
  • Press S on the keyboard to open the Model Toolbox and search for the Offset tool. Press Enter or click Offset to select the tool.

38- With the Offset tool active, click any edge of the top face. This should pick up all four edges.

39- Set the Offset position to -5 mm. You can also drag the blue slider to set the offset to -5 mm. This will create a sketch that is offset inside of the outer edge of the face. It will also be properly constrained because it is entirely dependent on the outer edge of the face.

40- Notice that we can still edit the 5 mm used for the offset. Double click the “5.00” dimension to edit the value. Move your mouse over the entry box and notice the value “d6: 5.00 mm”. The model assigns the 5 mm dimension to a variable to a variable, d6, that we can use in other parts of the model.

41- The sketch is now ready to be used in other parts of the model. Click Stop Sketch to exit the sketch.

42- Return to the Home view to better show the cut we will be making in the next steps.

43- The Extrude tool can also be used to remove material from a model. To imitate the shell, we will need to use the tool to do the following.

  • Remove material below the area created by the sketch that is offset from the outer edge of the box.
  • Remove material to a depth that offset the same distance from the bottom of the cube as the offset is from the sides.

44- Select the Extrude tool again and click on the inner area created by our offset sketch.

45- Change the Extrude Operation from New Body to Cut.

46- Because we want the depth of the cut to change depending on the thickness of the offset, we want to offset the cut the same distance from the bottom as the distance from the cut to the outer edge (5 mm).

47- Change Extrude Extent to To Object.

48- Rotate the model so you can see the bottom face of the model. You can do this by holding Shift+Middle Mouse Button to orbit or by clicking the corresponding corner of the View Cube.

49- Click on the bottom face of the model. Change the Extrude Offset to “-d6” to offset the cut the same distance as the distance between our cut and the outside wall.

50- Verify that your parameters match the screenshot below.

51- Click OK to submit the extruded cut. Return to the Home view on the ViewCube to see the cavity similar to the Shell tool.

52- Next we want to make a circular cut from the front left face of the box through the model to the opposite face.

53- Select Create Sketch and click on the front left face of the cube to set the sketch plane. This will reorient the window so we are looking perpendicular on the front left face of the box.

 

54- Select the Center Diameter Circle tool in order to create a circle based on the center and a set diameter. You can do this a few ways.

  • Click the Center Diameter Circle tool shortcut in the Toolbar.
  • Press C on the keyboard.
  • Click Sketch to open the Sketch palette and in the Circle submenu, click the Center Diameter Circle
  • Press S on the keyboard to open the Model Toolbox and search for the Center Diameter Circle tool. Press Enter or click Center Diameter Circle to select the tool.

55- Click once to set the center of the circle and click again to set the diameter. Make sure the circle is in the middle of the face. Notice the circle is Unconstrained.

56- We will need to use Construction Lines to ensure the center of the circle is in the center of the face. Similar to the Center Rectangle, we can create a Construction Line from one corner of the face to the other. The midpoint of this line will be the center of the face.

57- Select the Line tool in order to create a line that we can use for reference purposes. You can do this a few ways.

  • Click the Line tool shortcut in the Toolbar.
  • Press L on the keyboard.
  • Click Sketch to open the Sketch palette and click the Line
  • Press S on the keyboard to open the Model Toolbox and search for the Line tool. Press Enter or click Line to select the tool.

58- Click once on the upper left corner of the face, then click on the bottom right corner of the face. This will create a line that is properly Constrained because it references the endpoints of the line on the corners of the face.

59- The line is currently dividing the circle. We need to change this to a Construction Line to ensure it does not interfere with any features that use this sketch. To convert the line to a Construction Line, select the line and do one of the following.

  • In the Sketch Palette under Contextual Options, click Normal/Construction to toggle the line between Normal and Construction.
  • Press X on your keyboard. This is the keyboard shortcut for converting back and forth between Normal and Construction Lines.

60- With the Construction Line selected, hold Shift and click on the center of the circle. Click on Constraints in the Sketch Palette to show all available constraints between the construction line and the point at the center of the circle.

61- Select Midpoint. This will change the center of the circle from a white dot to black meaning it is properly Constrained.

62- The diameter of the circle has not been constrained yet. Select the Sketch Dimension tool and click on the edge of the circle. Dimension the circle diameter 20 mm. The sketch should be properly constrained.

63- The sketch is now ready to be used in other parts of the model. Click Stop Sketch to exit the sketch.

64- Return to the Home view to better show the cut we will be making in the next steps.

65- We will use an Extrude Cut and use the circle sketch to make a circular cut through the model. Select the Extrude tool again and click on the inner area of the circle.

66- Change the Extrude Operation from New Body to Cut.

67- Because we want the depth of the cut to extend through the entirety of the model, change Extrude Extent to All.

68- Change the direction of the cut to go back through the model.

69- Verify that your parameters match the screenshot below.

70- Click OK to submit the extruded cut. The component should be identical to the component from Lesson 3, Step 7.

71- Notice in the Timeline that each feature that took a single tool in Lesson 3 took both a sketch and a tool feature in Lesson 4. The timeline shows the sketches and the features that were created based on the sketches.

72- To make the edits that we did in Lesson 3, changes will need to be made to either the sketches or the features using the sketches. We made the following edits after completing the model in Lesson 3.

  • Change Box height from 40 mm to 25 mm.
  • Change Shell thickness from 5 mm to 2 mm.
  • Change Hole diameter from 20 mm to 15 mm.

73- To imitate the changes to the Box feature, the height was specified in the Extrude1 feature. Right-click on the Extrude1 feature in the timeline and click Edit Feature.

74- Change the Extrude Distance to 25 mm.

75- Click OK to submit changes. Note that the extruded circular cut is still in the middle of the face, and the diameter is too large for the new extruded height.

76- To imitate the Shell feature, the offset dimension was defined in Sketch2 to be 5 mm. To change the offset distance, we will need to edit Sketch2. Right-click on the Sketch2 sketch in the timeline and click Edit Sketch. You can also right-click on Sketch2 in the Browser under the Sketches folder.

77- Change the offset dimension to 2 mm. Double click on the dimension “5.00” and enter 2 mm. This will update the sketch.

78-Click Stop Sketch to update the changes to the sketch. Because we specified the offset of the depth of our cavity using the offset dimension d6 that was changed to 2 mm, the depth of the cavity automatically updated to this value.

79-Lastly, we need to change the diameter of the circular extruded cut. To imitate the Hole, the circular extruded cut was defined in Sketch3 to have a diameter of 20 mm. To change the diameter, we will need to edit Sketch3. Right-click on the Sketch3 sketch in the timeline and click Edit Sketch. You can also right-click on Sketch3 in the Browser under the Sketches folder.

80- Change the dimension from 20 mm to 15 mm.

81- Click Stop Sketch to update the changes to the sketch. Notice the greater distance between the bottom edge of the circular extruded cut and the bottom of the cavity.

82- Save your part using the Save button in the Application Bar at the top right of the window or by pressing Crtl+S on your keyboard. Leave the version description as User Saved and click OK to save the model.

83- You now have a finished part using Sketches in conjunction with tools like Extrude. This should be an identical component to the final component of Lesson 3. Sketching takes significantly more time for simple components like the completed part below, but it is necessary for more advanced functionality.

This concludes Lesson 4. You should now be able to do the following to use sketches along with tools to create and edit model features.

  • Identify use cases for Sketch tools.
  • Use Browser and Timeline to identify and edit sketches associated with features..
  • Edit sketches associated with features after they have been created.

Leave a Reply

Your email address will not be published. Required fields are marked *