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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
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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
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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
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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
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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
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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
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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
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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
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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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