Autodesk Fusion 360 模型创建教程说明书

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Lesson: Model creation

In this lesson, you’ll cover several important

topics when modeling for Generative

Design.

Learning Objectives

•

•

•

•

Create a fully dimensioned and

constrained sketch.

Create a 3D model using features.

Modify a model with fillets and

chamfers.

Use surfaces to create or patch

complex shapes.

The completed exercise

and open the supplied Lofted Bodies.f3d

and Under Defined Flange.f3d files.

te to the Toolbar’s Surface tab.

Page | 1

3. Rotate the model to the left view and notice that

the body’s hole is tapered.

4. Use the drop-down menu in the Toolbar’s

Create group to choose Create> Patch.

5. For the Patch dialog’s Boundary Edges

selection, choose the larger opening on the

body’s left face. A filled surface is created inside

the hole’s perimeter.

6. If needed, the dialog’s menu can be used to

change how the patch continues the body’s

curvature. In this instance, none of these options

are needed because the body has no curvature.

However, this tool does not allow you to select

the second edge to create a patch between the

two selections. An internal face cannot be

created between the two holes in the body’s

surfaces. Cancel the dialog.

Lesson: Model Creation

Page | 2

7. Click Create> Loft.

8. For the dialog’s Profile’s selections, choose the

two holes’ parameters. After the second

selection is made, the tapered face is previewed

in the Canvas. However, a non-tapered face

with a chamfer is needed to patch the holes.

Cancel the dialog.

9. Click Create> Extrude.

10. For the dialog’s Profile selection, choose the

smaller hole’s perimeter.

Lesson: Model Creation

Page | 3

11. Use the on-screen manipulator to drag the

selection through the part.

12. Choose the To Object option from the dialog’s

Extent menu.

13. Select the body’s face to extrude the selection

up to this face. These selections are

parametrically linked; if the model’s width

changes, then the extrusion distance will

automatically update.

14. The gap between the existing hole and the new

extrusion needs to be filled. Click Modify>

Extend. Select the hole’s perimeter as the

dialog’s Edges selection, then use the on-screen

manipulator to drag the selection inwards 2 mm.

Click OK in the dialog to accept the edge

extension.

15. Expand the Browser’s Bodies folder and notice

that there are two surface bodies listed in the

folder: the original body and the new extrusion

you created in Step 11.

Lesson: Model Creation

Page | 4

16. To join the two surface bodies into a single

body, click Modify> Stitch. For the dialog’s Stitch

Surfaces selections, choose the original surface

body and the new extruded face. A green

highlight shows where two edges meet. In this

instance, the extrusion meets the original body

on both faces. Red highlights indicate open

edges. OK the dialog.

17. The two surface bodies are joined and become

a solid body. The body’s icon in the Browser

changes to indicate that it is no longer a surface

body.

18. Click Create> Offset. For the Offset dialog’s

Faces/Surface Bodies selection, choose the

cylindrical face.

19. Use the on-screen manipulator to create a new

offset surface 5 mm inside the original selection,

then OK the dialog.

Lesson: Model Creation

Page | 5

20. Click Create> Thicken. Select the new offset

face as the dialog’s Faces selection, then use

the on-screen manipulator to thicken it outwards

until it meets the existing body. Make sure the

New Body option is selected in the dialog’s

Operation menu, then OK the dialog.

21. The second new solid body is added to the

Browser’s Bodies folder. The offset surface was

not absorbed during the creation of this new

solid body.

22. To remove the offset surface, select it in the

Browser, right-click it, then choose Remove from

the menu. This removes the surface body from

the folder and adds a Remove feature to the

timeline.

23. Return to the Toolbar’s Solid tab.

24. Expand the Browser’s Sketches folder and

notice the Bolt Pattern sketch has a pencil icon

next to it instead of a lock icon. This indicates

the sketch is not fully defined. Edit the sketch by

right-clicking it and choosing Edit Sketch from

the menu.

Lesson: Model Creation

Page | 6

25. The sketch currently has four circles that are not

fully defined and can be moved in the Canvas.

Their blue geometry indicates that they are not

fully defined. The top left circle has a dimension

attached to it. Constraints, construction

geometry, and dimensions can be used to fully

define these four circles.

26. Click Create> Sketch Dimension to open the

mention tool. Alternately, press the D key to use

the keyboard shortcut.

27. Add a dimension to the top right circle but don’t

enter a numeric value. With the new dimension’s

value field highlighted, click on the left circle’s 15

mm dimension and press Enter. The new

dimension is automatically linked to this original

dimension. If the original dimension changes,

the new dimension will automatically update to

match. This is one way to make sure the circles

stay the same diameter.

28. Click Constraints> Equal. An equal constraint

can be added between circles to make sure they

stay the same diameter. Select the original 15

mm circle, then select one of the circles that

does not have a dimension. An equal constraint

is added between these two circles. If one

circle’s diameter changes, the second will

automatically update. A small equal constraint

icon is added to the circles’ geometry to indicate

that they are equal to each other. Add an equal

constraint to make sure the last hole stays the

same diameter as the others.

Lesson: Model Creation

Page | 7

29. Click Constraints> Horizontal/Vertical. Select the

two top circles’ center points to add a horizontal

constraint between them. If one circle moves,

the second circle will automatically shift to stay

horizontal with it. Continue selecting the other

circles’ center points to make sure all the circles

are horizontal and vertical to each other.

30. Click Create> Line to open the Line tool.

Alternately, press L to use the keyboard

shortcut. In the dialog, activate the Construction

option so that the line will be drawn as a dashed

construction line. Use a horizontal line and a

vertical line to connect the top left circle’s center

point to the body’s edges.

31. Open the Equal constraint tool and select the

two construction lines. This will make sure they

stay equal to each other. Notice the other three

holes automatically shift to stay horizontal or

vertical the first hole. Open the Dimension tool

and add a 15 mm dimension to one of the

construction lines. The circle’s geometry turns

black to indicate that it is now fully defined.

However, the remaining three circles are not yet

fully defined.

32. Add a horizontal construction line connecting the

top right circle to the body’s right edge.

33. Add a vertical construction line connecting the

lower right circle to the body’s bottom edge.

Lesson: Model Creation

Page | 8

34. Add equal constraints between the two newest

construction lines and the original construction

line to drew in Step 30. The circles turn black to

indicate there fully defined.

35. Click Finish Sketch> Finish Sketch.

36. Turn on the visibility for the Bolt Pattern sketch

by clicking the eyeball icon next to it in the

Browser. Click Create> Extrude to open the

Extrude tool. Alternately, press E to use the

keyboard shortcut.

37. For the Extrude dialog’s Profile selections,

choose the four circles in the Bolt Pattern

sketch.

Lesson: Model Creation

Page | 9

38. Use the on-screen manipulator to extrude the

selections backwards through the part. In the

dialog’s Extent menu, choose the To Object

option. Choose the body’s back face as the

Object selection. The material will be removed

up to the selected face. OK the dialog to create

the four holes through the part.

39. Click Create> Sweep. Select the cylinder’s

outside face as the dialog’s Profile selection,

then choose the sketched line as the Path

selection. Choose the New Body option from the

Operation menu, then OK the dialog.

40. Navigate to the front view and notice there is a

pinch point on the sweep.

41. In the Browser’s Sketches folder, select Sweep

Path, right-click it, then choose Show

Dimension. Increase the path’s radius to 30 mm

and notice that the swept body automatically

updates to match the new path geometry. Turn

off the sketch’s visibility by clicking the eyeball

icon next to it in the Browser.

Lesson: Model Creation

Page | 10

42. In the Browser, turn on the visibility for the Key

Cut sketch. Edit the sketch. Turn off the visibility

for any bodies inside the Bodies folder and

notice that the sketch’s projected edge allows

you to select a closed region. Turn on the

visibility for the bodies and finish the current

sketch. Turn off the visibility for the Key Cut

sketch. Save the file.

43. Navigate to the Lofted Bodies tab. Click Create>

Loft.

44. Select the top and bottom rounded rectangles

as the dialog’s Profile’s selections.

45. For the dialog’s Rails selections, click the plus

icon inside the Rails section, then select the two

curved sketch entities in the Canvas.

Lesson: Model Creation

Page | 11

46. In the Browser, expand the Sketches folder and

turn on the visibility for the Guide 2 sketch. Add

the two curved sketch lines in the sketch as rails

for the loft. OK the dialog and inspect the new

geometry.

47. Use the Browser to turn on the visibility for the

Split Profile sketch, then click Modify> Split

Body. For the dialog’s Body to Split option,

choose the lofted body you just created. For the

Splitting Tool selection, choose the Split Profile

sketch.

48. The splitting tool splits all the way through the

entire body. This was not the intended effect, so

Cancel the dialog.

49. Click Modify> Split Face. Make the same

selections you made in Step 47, then OK the

dialog. The body remains a single body, but the

top face is split by the selection.

50. Click Modify> Combine. For the dialog’s Target

Body selection, choose the lofted body. For the

Tool Bodies selection, choose the Plug body.

Make sure the Cut option is selected from the

Operation menu, then activate the Keep Tools

option. OK the dialog. The Plug body cuts the

geometry from the lofted body but is not

consumed by the operation.

Lesson: Model Creation

Page | 12

51. Click Modify> Shell. For the dialog’s Faces/Body

selection, choose the lofted body’s face you split

in Step 49. Specify a 2 mm wall thickness, then

OK the dialog.

52. Rotate the body and notice that the entire lofted

body now has a 2 mm wall thickness. Save the

file and continue to the next module.

Lesson: Model Creation

Page | 13

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