The document provides instructions for modeling the body of an F1 race car in SolidWorks. It involves creating several extruded cuts and a loft feature. Key steps include: 1) Creating a side cut by extruding a sketched profile. 2) Adding a rear cut by extruding another sketched profile. 3) Cutting out the top of the body by extruding a mirrored sketch. 4) Using a loft to model the cockpit area between two sketches on different planes. 5) Adding more cuts and lofts to further define the body shape.

1. F1 Car
Chapter 2
Body
A. Save as "BODY".
Step 1. If necessary, open your BLANK file.
Step 2. Click File Menu > Save As.
Step 3. Key-in BODY for the filename and
press ENTER.
B. Side Cut.
Step 1. Click Wireframe on the View toolbar.
Fig. 1
Step 2. Click Right (plane) in the Feature Manager and click Sketch from the Content
toolbar, Fig. 1.
Step 3. Click Normal To on the Standard Views toolbar. (Ctrl-8)
Step 4. Click Line (L) on the Sketch toolbar.
)
Step 5. Draw the 4 lines in Fig. 22.
Keep the lines away from
the cartridge hole. Use
the inferencing line, the
dotted line that appears
when you draw the Fig. 2
lines.
Step 6. Click Spline (S) Spline
on the Sketch toolbar.
Step 7. Draw a spline across Fig. 3
the top, Fig. 3. Press
Escape to end the
spline.
Control Point
Step 8. Click the spline to dis-
play the Spline Points
(green) and Control
Polygon. Fig. 4
Step 9. Click a gray Control Point to activate it and the Control Point turns yellow. Move the yel-
low Control Point to adjust spline, Fig. 4.
10/16/09
SolidWorks 08 Body F1 CAR Page 2-1
Brookside Middle School Tech Ed
http://www.sarasota.k12.fl.us/brookside/cudacountry email:cudacountry@comcast.net

2. Step 10. Click Smart Dimen-
sion (S) on
the Sketch toolbar.
Step 11. Dimension as shown
Fig. 5. To Smart di- Fig. 5
mension click the line to dimension, then move the cursor up off the sketch and click. Key-
in the dimension and press ENTER. To Smart dimension the over all length, 195, click the
back corner and click the front line. Move the cursor up off the sketch and click. Key-in
195 for the dimension and press ENTER.
Step 12. Click Features on the Command Direction arrow
Manager toolbar.
Step 13. Click Extruded Cut on the Features Fig. 7
toolbar.
Step 14. In the Extrude Property Manager:
under Direction 1
End Condition to Through All
The Direction arrow should
point towards area to be cut away,
Fig. 7. If arrow is pointing in wrong
direction, click Flip side to cut, Fig. 6.
Click OK
Fig. 6 Fig. 8
Step 15. Save. Use Ctrl-S.
C. Rear Cut. Back face
Step 1. Click Back on the Standard Views toolbar. (Ctrl-2)
Step 2. Click the back face of the body and click Sketch on
the Content menu, Fig. 9.
Step 3. Click Centerpoint Arc (S) in the Arc flyout
on the Sketch toolbar.
Fig. 9
SolidWorks 08 Body F1 CAR Page 2-2

3. Step 4. Start arc at center of the cartridge hole and move
3. Drag around
the cursor to the right. Click to place the first end and click to 2. Click
point, then move cursor counterclockwise 180 de- end arc end point
grees. Click to place the second end point, Fig. 10.
Step 5. Click Line (L) on the Sketch toolbar. 1. Start at
axle center
Step 6. Draw the 4 lines in Fig. 11. Start the line at the end
of the arc. Use the inferencing line, the dotted line Fig. 10
that appears when you draw the lines.
Step 7. Click Smart Dimension (S) on the Sketch
toolbar.
Step 8. Dimension arc 13, Fig. 12.
Step 9. Click Features on the Command
Manager toolbar. Fig. 11
Step 10. Click Extruded Cut on the Features
toolbar. Direction
arrow
Step 11. In the Extrude Property Manager:
under Direction 1
End Condition to Through All
The Direction arrow should point towards
area to be cut away, Fig. 13. If arrow is pointing in Fig. 12
wrong direction, click Flip side to cut, Fig. 14.
Click OK .
Step 12. Click Isometric on the Stan-
dard Views toolbar.
Step 13. Save. Use Ctrl-S.
Fig. 13 Fig. 14
SolidWorks 08 Body F1 CAR Page 2-3

4. D. Top Cut.
Top face
Step 1. Click the top flat face of the body and click Sketch
on the Content menu, Fig. 15.
Step 2. Click Normal To on the Standard Views toolbar.
(Ctrl-8)
Step 3. Click Centerline in the Line flyout (S) on Fig. 15
the Sketch toolbar.
Step 4. Starting from midpoint of the bottom of
the sketch, draw a centerline up through
the sketch, Fig. 16.
Step 5. Press the Escape key to unselect Cen-
terline.
Step 6. Click the centerline to select it, Fig. 16.
Centerline
Step 7. Click Dynamic Mirror on the
Sketch toolbar or Tools Menu > Sketch
Tools > Dynamic Mirror, Fig. 16.
Symmetry symbols appear at both ends
of the centerline. Geometry drawn on
one side of mirror centerline will mirror
onto the other side. Dynamic
Mirror
Step 8. Click Line (L) on the Sketch Fig. 16 Fig. 17
toolbar.
Step 9. Draw the 5 lines in Fig. 17. Keep the vertical line away from the blank. Avoid any infer-
encing lines except vertical.
SolidWorks 08 Body F1 CAR Page 2-4

5. Step 10. Click Smart Dimension
(S) on the Sketch toolbar.
Step 11. Add dimensions as shown
in Fig. 18. Start at the top,
with the 40. Dimension the
distance between the side pod
edge and the edge of Blank 2.
1
2
Step 12. Click Tangent Arc in Fig. 19
the Arc flyout on the
Sketch toolbar.
Step 13. Draw an arc between the Posi-
tion 1 and Position 2, Fig. 19.
Step 14. Click Features on the Fig. 18
Command Manager toolbar.
Step 15. Click Extruded Cut on the
Features toolbar. Direction
arrow
Step 16. In the Extrude Property Manager:
under Direction 1
End Condition to Through All
The Direction arrow should
point towards area to be cut away,
Fig. 20. If arrow is pointing in wrong
direction, click Flip side to cut, Fig. 21.
Fig. 20 Fig. 21
Click OK .
Step 17. Click Isometric on the Standard Views toolbar.
Step 18. Click Shaded With Edges on the View toolbar.
Step 19. Save. Use Ctrl-S.
Fig. 22
SolidWorks 08 Body F1 CAR Page 2-5

6. E. Under Front Wheel Cut.
Step 1. Rename Features in the Feature Manager (left panel). To rename,
click the Feature name and press F2, Fig. 23.
Change: BODY
CARTRIDGE HOLE
AXLE HOLES
EYE SCREW SLOT
SIDE CUT
REAR CUT
TOP CUT
Fig. 23
Step 2. Click Right (plane) in the Feature Manager and click Sketch from the Content
toolbar, Fig. 23.
Step 3. Click Normal To on the Standard Views toolbar. (Ctrl-8)
Step 4. Click Spline (S) on the Sketch toolbar.
Step 5. Draw a 3 point spline across the bottom in front of the axle, Fig. 24. Allow room for the
front wing, above and between the spline and the nose tip. Also, allow for the wheel stand-
offs around the axle hole. Press Escape
to end the spline. Point 2
Point 1
Step 6. Click the spline to display the Spline Point 3
Points (green) and Control Polygon. Fig. 24
Step 7. Click a gray Control Point to activate it
and the Control Point turns yellow. Move
the yellow Control Point to adjust spline,
Fig. 25.
Fig. 25
Step 8. Click Features Direction
on the Command Manager arrow
toolbar.
Step 9. Click Extruded Cut Fig. 26
on the Features toolbar.
Step 10. In the Extrude Property Man-
ager:
under Direction 1
End Condition to Through All Fig. 27 Fig. 28
The Direction arrow should point towards area to be cut away, Fig. 26. If arrow
is pointing in wrong direction, click Flip side to cut, Fig. 27. Click OK .
SolidWorks 08 Body F1 CAR Page 2-6

7. F. Loft Cockpit.
Step 1. Rename Features in the Feature
Manager. To rename, click the
Feature name and press F2, Fig. 29.
Change:
Extrude 4 to FRONT WHEEL
Top face
CUT.
Step 2. Click the top face of the body and
click Sketch on the Content
Fig. 29
menu, Fig. 30.
Fig. 30
Step 3. Click Normal To on the Standard
Views toolbar. (Ctrl-8)
Step 4. Click Zoom to Selection (Q) on the
View toolbar to zoom around the front of
cockpit, Fig. 31.
Step 5. Click Centerline in the Line flyout
(S) on the Sketch toolbar.
Zoom
Step 6. Starting from midpoint of the cartridge arc Centerline
edge, draw a centerline down through the
sketch, Fig. 32.
Dynamic
Step 8. With the centerline selected, click Dynamic Mirror
Mirror on the Sketch toolbar or Fig. 31 Fig. 32
Tools Menu > Sketch Tools > Dynamic Mirror, Fig. 32.
Position 1
Position 2
Step 9. Click Line (L) on the Sketch toolbar.
Step 10. Draw the 2 lines in Fig. 33. Start the first line at top
endpoint of centerline, Position 1, Fig. 33. Bring the Position 3
line over to the corner, Position 2. Continue another line
down vertically, Position 3.
Step 11. Click Spline (S) on the Sketch toolbar.
Fig. 33
SolidWorks 08 Body F1 CAR Page 2-7

8. Step 12. Draw a spline from the end of the vertical line to the center-
line, Fig. 34. Press Escape to end the spline.
Step 13. Shift click a vertical line and a spline to select both, Fig. 34. Line
To Shift click, click a vertical line, then hold down the Shift
key and click the spline.
Spline
Step 14. Click Tangent on the Content menu, Fig. 35.
Fig. 34
Step 15. Click a gray Control Point to activate it and the Control Point
turns yellow. Move the yellow Control Point to adjust spline,
Fig. 35.
Step 16. Click Smart Dimension (S) on the Sketch toolbar.
Step 17. Dimension as shown Fig. 36.
Step 18. Click Exit Sketch on the Sketch toolbar.
Fig. 35
Step 19. Click Isometric on the Standard Views toolbar.
Step 20. Click the top face of the body, Fig. 37.
Step 21. Click Insert Menu > Reference Geometry > Plane.
Step 22. In the Plane Property Manager, under Selections:
Set Offset Distance to 7
click OK in the Property Manager, Fig. 38. Fig. 36
Top face
Fig. 37
Fig. 38
SolidWorks 08 Body F1 CAR Page 2-8

9. Step 23. Click the cockpit sketch (Sketch 9) in the Feature
Manager, Fig. 39 and copy. Use Ctrl-C to copy
sketch.
Step 24. Click the new Plane (Plane1) in the Feature Man-
ager, Fig. 40 and paste sketch. Use Ctrl-V to paste
sketch, Fig. 41.
Step 25. Click the Sketch10 (pasted sketch) in the Feature
Manager and click Edit Sketch on the Con-
tent menu, Fig. 41.
Fig. 39 Fig. 40
Step 26. Click Normal To on the Standard Views toolbar.
(Ctrl-8)
Step 27. Click Zoom to Selection
(Q) on the View toolbar to zoom Sketch
around cockpit.
Step 28. Click the top left corner of the
sketch and click Make Fixed
on the Content menu,
Fig. 42. Fig. 41
Fig. 42
Step 29. Change dimension of line
Click corner
from 23 to 14, Fig. 43. to fix
Step 30. Click Exit Sketch on
the Sketch toolbar.
Fig. 43 Fig. 44
SolidWorks 08 Body F1 CAR Page 2-9

10. Step 31. Click Isometric on the Standard Views toolbar.
Step 32. Click Loft Base/Boss on the Features toolbar.
Step 33. Click both sketches, Fig. 45.
Step 34. In the Loft Property Manager, Sketch
under Options check Merge
results, Fig. 46 and click OK Sketch
.
G. Create Folder for Loft. Fig. 45
Step 1. Click the Plane1 in the Feature
Fig. 46
Manager and click Hide
on the Content menu, Fig. 47.
Step 2. Shift click Plane1 and Loft1
in the Feature Manager to
select both. Right click and
click Add to New Folder on
the menu, Fig. 48.
Step 3. Rename new Folder LOFT
COCKPIT in the Feature
Manager. To rename, click the Fig. 49
Folder name and press F2, Fig. 49.
Fig. 47
Fig. 48
H. Loft Cartridge Front.
Step 1. Click the front face of the cartridge hole arc and click Sketch on the Content menu,
Fig. 50.
Step 2. With the front face still selected, click Convert Entities
on the Sketch toolbar.
Front face
Step 3. Click Exit Sketch on the Sketch toolbar.
Fig. 50
SolidWorks 08 Body F1 CAR Page 2-10

11. Step 4. Click the top face of cockpit loft and click Sketch
on the Content menu, Fig. 51.
Top face
Step 5. Click Normal To on the Standard Views
toolbar. (Ctrl-8)
Step 6. Click Zoom to Selection (Q) on the View
toolbar to zoom around the front of cockpit, Fig. 52.
cockpit
Fig. 51
Step 7. Click Centerline in the Line
flyout (S) on the Sketch
toolbar. Dynamic
Mirror
Step 8. Starting from midpoint of the car- Centerline
tridge arc edge, draw a centerline
down through the sketch, Fig. 53. Zoom
Step 9. With the centerline selected, click
Dynamic Mirror on the Fig. 53
Position 1
Sketch toolbar or Tools Menu > Position 2
Sketch Tools > Dynamic Mirror,
Fig. 53. Symmetry symbols appear Position 3
Fig. 52
at both ends of the centerline. Geometry drawn on
one side of mirror centerline will mirror onto the other
side.
Step 10. Click Line (L) on the Sketch toolbar.
Step 11. Start first line top endpoint of centerline , Position 1,
Fig. 54. Bring the line over to the corner, Position 2. Fig. 54
Continue another line down vertically, Position 3. The
lines will mirror over to the other side of the Dynamic
Mirror centerline.
Start arc
Step 12. Click Centerpoint Arc (S) in the Arc flyout
on the Sketch toolbar.
Step 13. Start arc on centerline aligned with the end of verti-
cal line and move the cursor to the left. Click to place
the first end point, then move cursor counterclockwise Fig. 55
90 degrees. Click to place the second end point, Fig. 55.
SolidWorks 08 Body F1 CAR Page 2-11

12. Step 14. Click Smart Dimension (S) on the Sketch
toolbar.
Step 15. Dimension line 11 and arc radius 13 as shown in
Fig. 56.
Step 16. Click Exit Sketch on the Sketch toolbar.
Step 17. Click Isometric on the Standard Views toolbar. Fig. 56
Step 18. Click Loft Base/Boss on the Features toolbar.
Step 19. Click the offset entities sketch and the sketch on top face, Fig. 57.
Step 20. In the Loft Property Manager,
under Start/End Constraints:
Set Start constraint:
Tangency to Face Sketch 1
Set Start Tangent Length: .9
Fig. 57 and Fig. 58 Sketch 2
click OK in the Prop-
erty Manager.
Fig. 57
Step 21. Save. Use Ctrl-S.
I. Create Side Pod Construction Sketch.
Step 1. Click the side face of body (side pod), Fig. 59.
Step 2. Click Insert Menu > Surface > Offset. Fig. 58
Step 3. In the Property Manager, set:
Offset distance to 3,
Fig. 60 and click OK .
Side face
Fig. 59 Fig. 60
SolidWorks 08 Body F1 CAR Page 2-12

13. Step 4. Click the new surface and click Sketch on the
Content menu, Fig. 61.
Step 5. Click Offset Entities on the Sketch toolbar.
Step 6. In the Offset Entities Property Manager set:
Distance to 3 Surface
The yellow offset rectangle should be on the out- Fig. 61
side of the face, Fig. 62. If it is not, click Reverse.
Click OK .
Step 7. Click Surface-Offset1 in the Feature Manager and
click Hide on the Content menu, Fig. 63 and
Fig. 64.
Step 8. Click Exit Sketch on the Sketch toolbar.
J. Create Side Pod 3D Sketch.
Step 1. Use the Rotate View in the View toolbar to
rotate view as shown in Fig. 64. Fig. 62 Fig. 63
Step 2. Use the Zoom to Area in the View toolbar
to drag a zoom window around the left side pod,
Fig. 64.
Step 3. Click 3D Sketch in the Sketch
Zoom
flyout on the Sketch toolbar. Be sure to click Fig. 64
the flyout arrow to select 3D Sketch.
Step 4. Click Spline (S) on the Sketch toolbar.
)
1
The cursor should change to XY plane
indicating you are sketching in XY plane. If
not, press Tab to switch sketch plane.
Step 5. Click to start spline at the top corner (vertex)
of body and side pod, Position 1, Fig. 65.
Fig. 65 2
Step 6. Click 2nd endpoint of spline on the back vertical line of the 2D sketch, Position 2. Keep
the endpoint away from the midpoint of the line. Press Escape to end Spline, Fig. 65.
SolidWorks 08 Body F1 CAR Page 2-13

14. Step 7. Press S key again and select Spline .
Step 8. Press Tab to change the sketch plane to the
3
YZ plane . View the Reference Triad
at the bottom left corner of the display Fig. 66 2
to determine the sketch plane.
Step 9. Draw a spline from Position 2 on the back 4
vertical line of 2D sketch to front vertical
line, Position 3, Fig. 66. Press Escape to
end Spline. 3
Step 10. Press S key again and select Spline .
Step 11. Use the right arrow to rotate view as shown
in Fig. 67. Fig. 67
Step 12. Draw a spline from Position 3 on the front
4
vertical line of 2D sketch to top corner (ver-
tex) of body and side pod, Position 4, Fig.
67. Press Escape to end Spline. 1
Step 13. Click Line (L) on the Sketch toolbar.
Step 14. Draw a line across the top of the body to con-
nect the ends of the splines, Position 1 to Fig. 68
Position 4, Fig. 68. Press the Escape key to
unselect Line.
Step 15. Click Smart Dimension (S) on the
Sketch toolbar.
Step 16. Add dimensions between endpoints of
spline and top corner of the 2D sketch as
shown in Fig. 69. To Smart dimension, the
end of spline point and the top corner of 2D Fig. 69
sketch.
SolidWorks 08 Body F1 CAR Page 2-14

15. Step 17. Press the Escape key to unselect Smart Dimension.
Step 18. Click Back on the Standard Views toolbar. (Ctrl-2)
Step 19. Click the lower spline to display the Spline Points (green)
and Control Polygon.
Step 20. Click a gray Control Point to activate it and the Control Fig. 70
Point turns yellow. Move the yellow Control Point to adjust spline, Fig. 70.
Step 21. Click Right on the Standard Views
toolbar. (Ctrl-4)
Step 22. Use the Control Points to adjust spline,
Fig. 71.
Step 23. Click Front on the Standard Views Fig. 71
toolbar. (Ctrl-1)
Step 24. Use the Control Points to adjust top spline, Fig. 72.
Step 25. Be careful when adjusting the splines. The splines must
be keep out away from the body or the surface created
from this 3D sketch will not cut the body. Avoid this er-
ror by adjusting spline in each view (Normals). Check
splines in top view. Fig. 73 is correct, but Fig. 74 has
Fig. 72
error.
Keep splines
outside body
Step 26. Click Isometric on the Standard
Views toolbar.
Step 27. Exit the 3D Sketch. To Exit, click
in the Sketch flyout on
the Sketch toolbar. Click the flyout arrow
then 3D Sketch.
Fig. 73 Fig. 74
SolidWorks 08 Body F1 CAR Page 2-15

16. K. Create Fill Surface.
Step 1. Click Insert Menu > Surface >
Fill.
Step 2. Select the 3D Sketch, Fig. 75.
Click OK in the Property
Manager, Fig. 76. 3D Sketch
L. Cut with Surface. Fig. 75
Step 1. Click Insert Menu > Cut > With Surface.
Step 2. In the SurfaceCut Property Manager:
click cut surface in drawing, Fig. 77
77. Fig. 76
the Direction arrow should point
towards area to be cut way, Fig. 77
if arrow is pointing in wrong
direction, click Flip Cut
, Fig. 78 Direction
arrow
click OK . Surface
Fig. 77 Fig. 78
Step 3. Click Surface-Fill1 in Feature
Manager and click Hide on the Content menu, Fig. 79.
Step 4. Expand Surface-Fill1 in Feature Manager, click 3DSketch1 and click Hide on the
Content menu, Fig. 80.
M. Copy Side Pod 3D Sketch.
Step 1. Click 3DSketch1 in the Feature Manager, Fig. 81.
Step 2. With the 3D Sketch selected, use Ctrl-C to copy 3D
Sketch.
Step 3. Use Ctrl-V to paste 3D Sketch. Fig. 79
Fig. 80
Step 4. Click the new copied 3D Sketch in the Feature
Manager and click Edit Sketch on the Content
menu, Fig. 82.
Fig. 81
Fig. 82
SolidWorks 08 Body F1 CAR Page 2-16

17. Step 5. Click Isometric on the Standard
Views toolbar.
Zoom
Step 6. Rotate View and Zoom to Area
Fig. 83
around side pod, Fig. 83.
Step 7. Pull down the vertex at the top corners of
line and spline, Positions 1 and 4 down
to the bottom of body, Fig. 84. Keep the
vertex in the corner (edge). If the vertex is
not at the bottom the surface will not cut.
4
Pull vertex
of spline down
Step 8. Click Smart Dimension (S) on to bottom Fig. 84 1
the Sketch toolbar.
Step 9. Change the front dimension to 20 and the
back dimension to 23 at the corners be-
tween endpoints of spline and top corner of
the 2D sketch as shown in Fig. 85.
Step 10. Press the Escape key to unselect Smart
Dimension.
Fig. 85
Step 11. Click Back on the Standard Views toolbar. (Ctrl-2)
Keep splines
Step 12. Click the bottom spline to dis- outside body
play the Spline Points (green)
and Control Polygon.
Step 13. Click a gray Control Point
to activate it and the Control
Point turns yellow. Move the Fig. 86
yellow Control Point to adjust
spline, Fig. 86.
Step 14. Click Front on the Stan-
dard Views toolbar. (Ctrl-1)
Step 15. Use the Control Points to ad-
just spline, Fig. 87. Fig. 87 Fig. 88
Step 16. Check the splines in the Top View , Fig. 88. The splines most be outside the body or
the surface created from this 3D sketch will not cut the body.
SolidWorks 08 Body F1 CAR Page 2-17

18. Step 17. Click Isometric on the Standard Views toolbar.
Step 18. Exit the 3D Sketch. To Exit, click in the Sketch flyout on the Sketch
toolbar. Click the flyout arrow then 3D Sketch.
N. Create Lower Fill Surface.
Step 1. Click Insert Menu > Surface > Fill.
Step 2. Select the 3D Sketch, Fig. 89.
Click OK in the Property
Manager, Fig. 90.
O. Cut with Lower Surface. 3D Sketch
Step 1. Click Insert Menu > Cut > With
Surface. Fig. 89
Step 2. In the SurfaceCut Property Manager:
click cut surface in drawing, Fig. 91
91.
the Direction arrow should point Fig. 90
towards area to be cut away,
Fig. 91
if arrow is pointing in
wrong direction, click
Direction
Flip Cut , Fig. 92 arrow
Surface Fig. 92
click OK . Fig. 91
Step 4. Click Surface-Fill2 in Feature Manager and click Hide on the Content menu, Fig. 93.
Step 5. Click Sketch13 (2D rectangle sketch) in the Feature Manager and click Hide
on the Content menu, Fig. 94.
Fig. 93 Fig. 94
SolidWorks 08 Body F1 CAR Page 2-18

19. P. Mirror Side Pod.
Step 1. Click Mirror on the Features toolbar.
Step 2. In the Property Manager set:
under Mirror Face/Plane, Fig. 96
expand the Design Tree in the top left
corner of the drawing area
click Right (Plane), Fig. 97
under Features to Mirror
in Design Tree select
SurfaceCut1 and
SurfaceCut2
click OK , Fig. 98.
Step 3. Save. Use Ctrl-S. Fig. 96 Fig. 97
Step 4. In the Feature Manager
create folder for Side Pods. Fig. 98
To create folder select all
features. Click the first
feature, hold down Shift
key and click last feature,
Fig. 99.
Step 5. Right click any selected
feature and click Add to
New Folder on the Con-
tent menu (click OK to
warning) Fig. 100.
Step 6. Rename the folder SIDE Fig. 99 Fig. 100 Fig. 101
POD. To rename, select
folder and use F2 key, Fig. 101.
Q. Wheel Standoff.
Step 1. Click Right (plane) in the Feature Manager and click Sketch
from the Content toolbar, Fig. 102.
Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8)
Fig. 102
Step 3. Use the Zoom to Area in the
View toolbar to drag a zoom window
around the front axle hole, Fig. 103.
Zoom
Fig. 103
SolidWorks 08 Body F1 CAR Page 2-19

20. Step 4. Click the edge of the front axle hole, Fig. 104.
Convert edge to entities
Step 5. Click Convert Entities on the Sketch
toolbar.
Step 6. Click Centerline in the Line flyout (S)
on the Sketch toolbar. Fig. 104
Step 7. Draw two centerlines from the center of the circle
as shown in, Fig. 105. Keep one centerline horizon-
tal.
Horizontal center-
Step 8. Click Smart Dimension (S) on the Sketch
toolbar.
Fig. 105
Step 9. Dimension angle between construction lines 10 as
shown in Fig. 106. To Smart dimension click both
construction lines, then move the cursor and click.
Key-in 10 for the dimension and press ENTER.
Step 10. Click Ellipse on the Sketch toolbar. Horizontal center-
Step 11. Draw an ellipse as shown in Fig. 107. To draw el-
lipse, click the center of circle to place the center of Fig. 106
the ellipse. Drag to the angled center line and click
to set the major axis. Drag down below circle and
click again to set the minor axis. Major axis
Step 12. Click Smart Dimension (S) on the Sketch
toolbar.
Minor axis
Step 13. Dimension ellipse as shown in Fig. 108. To Smart
dimension click the major axis points, then move Fig. 107
the cursor up off the sketch and click. Key-in 17 for
the dimension and press ENTER. Dimension the
minor diameter 8.
Step 14. Save. Use Ctrl-S.
Fig. 108
SolidWorks 08 Body F1 CAR Page 2-20

21. Step 15. Zoom out, use the Z key and use
Zoom to Area to drag a
zoom window around the both
axle holes, Fig. 109.
Zoom
Step 16. Press Escape to unselect Zoom. Fig. 109
Step 17. Copy sketch to rear axle. To Drag selection
around sketch
copy, drag selection around
sketch, Fig. 110. Be sure to
get the dimensions in selection.
Hold down Ctrl key and drag
from center of axle hole (circle) Ctrl Drag Ctrl Drag to
to center of rear axle hole. from center Fig. 110 center of axle hole
Step 18. Click Features n the Command Manager toolbar.
Step 19. Use the Rotate View in the View toolbar to rotate view as shown in Fig. 111.
Step 20. Click Extruded Boss/Base
on the Features toolbar.
Step 21. In the Property Manager set:
under From
Start Condition to Offset
Offset Value to 3
under Direction 1
Depth to 16
click OK , Fig. 111 and Fig. 111 Fig. 112
Fig. 112.
Step 22. Rename the Extruded Feature WHEEL STANDOFF. To rename, se-
lect folder and use F2 key, Fig. 113.
Fig. 113
SolidWorks 08 Body F1 CAR Page 2-21

22. R Mirror Wheel Standoff.
Step 1. Click Mirror on the Features toolbar.
Step 2. In the Property Manager set:
under Mirror Face/Plane, Fig. 114
expand the Design Tree in the top left
corner of the drawing area
click Right (Plane), Fig. 115
under Features to Mirror
in Design Tree select
WHEEL STANDOFF Fig. 114
click OK , Fig. 116.
Fig. 115
Step 3. Save. Use Ctrl-S.
Fig. 116
S. Fillet Top Edges.
Step 1. Click Isometric on the
Standard Views toolbar. (Ctrl-7)
Step 2. Click Fillet on the Fea-
tures toolbar. Edge
Step 3. In the Fillet Property Manager:
Edge
Select FilletXpert, Fig. 117.
117 Fig. 118
Set the Radius to 3 Fig. 117
Click the inside edge on all 4
wheel standoffs on both sides
of the body (hold down middle Edge
mouse button to rotate view),
Fig. 118. Edge
Click Apply Fig. 120
Set the Radius to 1
Click the end edge on all 4
wheel standoffs, Fig. 120. Fig. 119
click OK , Fig. 121.
Fig. 121
SolidWorks 08 Body F1 CAR Page 2-22

23. T. Bottom Rear 3D Sketch. Snap to Centerline
vertex
Step 1. Click Back on the Standard Views toolbar.
(Ctrl-2)
Step 2. Click 3D Sketch in the Sketch flyout
on the Sketch toolbar.
Centerline Fig. 122
Start at
Step 3. Click Centerline in the Line flyout (S) midpoint
Draw arc
on the Sketch toolbar. beyond
center
of body
Step 4. Draw two centerlines as shown in Fig. 122. Snap
endpoint to the vertex.
Step 5. Click Centerpoint Arc (S) in the Arc flyout
Fig. 123
on the Sketch toolbar.
Step 6. Click the midpoint of top centerline (center of the
cartridge hole) to start the arc and move the cursor
to the left end of centerline. Click to place the first
endpoint, then move cursor counterclockwise past 90
degrees or beyond middle of body. Click to place the
second endpoint, Fig. 123.
Draw line
past centerline Fig. 124
Step 7. Click Line (L) on the Sketch toolbar.
Step 8. Draw the line as shown in Fig. 124. Start line at mid-
point of top centerline and continue line down past
bottom centerline (origin). Trim 3
Step 9. Click Trim Entities on the Sketch toolbar.
Fig. 125
Step 10. Trim the entities as shown in Fig. 126. To trim, click
the entities you want to remove, Fig. 125.
Fig. 126
SolidWorks 08 Body F1 CAR Page 2-23

24. Step 11. Press Escape to unselect Trim Entities.
Step 12. Use right arrow two times to rotate view as shown in 1
Fig. 127.
Step 13. Click 3 Point Arc on the Sketch toolbar.
3
Step 14. Press Tab to change the sketch plane to the YZ plane
2
. Fig. 127
Step 15. Draw an arc between the Position 1, Position 2 and Posi-
tion 3 shown in Fig. 127. To draw the arc, first click Posi-
tion 1, then Position 2. Swing the arc to Position 3 and
click. At Position 1 keep the arc inside the edge of the
body.
Step 16. Click Smart Dimension (S) on the Sketch
toolbar.
Fig. 128
Step 17. Dimension the endpoint of arc to the side pod 11 as shown Fig. 128
128.
Step 18. Use up arrow two to rotate view as shown in Fig. 129.
Step 19. Click 3 Point Arc on the Sketch toolbar.
Step 20. Change the sketch plane to ZX . Use the tab key. 3
The cursor will change to ZX.
1 2
Step 21. Draw an arc between the Position 1, Position 2 and Posi-
tion 3 to close the 3D Sketch as shown in Fig. 129. To Keep arc Fig. 129
inside edge
draw the arc, first click of body
Position 1, then Position
2. Swing the arc to Posi-
tion 3 and click. At Posi-
tion 1 keep the arc inside
the edge of the body, Fig.
130 and Fig.131.
Step 22. Exit the 3D Sketch. To
Exit, click
in the Sketch flyout Fig. 130 Keep arc Fig. 131
on the Sketch toolbar. Good inside edge Wrong
of body
SolidWorks 08 Body F1 CAR Page 2-24

25. U. Create Bottom Rear Fill Surface.
Step 1. Click Insert Menu > Surface > Fill.
3D Sketch
Step 2. Select the 3D Sketch, Fig. 132. Click
OK in the Property Manager,
Fig. 133.
V. Cut Bottom Rear Surface.
Step 1. Click Insert Menu > Cut > With Sur-
face. Fig. 132
Step 2. In the SurfaceCut Property Manager:
click cut surface in drawing, Fig. 133
Fig. 134
Direction
the Direction arrow should point arrow
towards area to be cut away,
Fig. 134
if arrow is pointing in wrong Surface
direction, click Flip Cut ,
Fig. 135
click OK .
Fig. 134 Fig. 135
Step 3. Click Surface-Fill3 in Feature Manager and click Hide on the
Content menu, Fig. 136. The 3DSketch3 should hide itself.
Fig. 136
SolidWorks 08 Body F1 CAR Page 2-25

26. W. Mirror Bottom Rear.
Step 1. Click Mirror on the Features toolbar.
Step 2. In the Property Manager set:
under Features to Mirror, Fig. 137
expand the Design Tree in the top left
corner of the drawing area
click Right (Plane), Fig. 138
under Features to Mirror
in Design Tree select
SurfaceCut3 Fig. 137
click OK , Fig. 138.
Step 3. In the Feature Manager create a folder
for BOTTOM REAR CUT. To cre-
ate folder, first select all features, click Fig. 138
the first feature, hold down Shift key
and click last feature, Surface-Fill3 to
Mirror3, Fig. 140.
Step 4. Right click any selected feature and Fig. 139
click Add to New Folder on the Con-
tent menu (click OK to
warning) Fig. 141.
Step 5. Rename the folder BOT-
TOM REAR CUT. To
rename, select folder and
use F2 key, Fig. 142.
Fig. 140
Fig. 141
Fig. 142
SolidWorks 08 Body F1 CAR Page 2-26

27. X. Front Wing.
Step 1. Click Right (plane) in the Feature Manager and click Sketch
from the Content toolbar, Fig. 143.
Step 2. Click Normal To on the Standard Views toolbar. (Ctrl-8)
Step 3. Use the Zoom to Area in the Fig. 143
View toolbar to drag a zoom window
around the area in front of front axle,
Fig. 144.
Zoom
Step 4. Click Line (L) on the Sketch Fig. 144
toolbar.
Step 5. Draw the 2 lines in Fig. 145. Keep one line hori-
zontal.
Step 6. Click Smart Dimension (S) on the
Sketch toolbar. Fig. 145
Step 7. Add the Dimensions as shown in Fig. 146. To
Smart dimension the angle click the middle of the
construction lines, then move the cursor and click.
Key-in 18 for the dimension and press ENTER.
Step 8. Click Offset Entities Fig. 146
on the Sketch toolbar.
Offset
Step 9. In the Offset Entities Property
Manager set:
Distance to 4
check Bi-directional
click the angled line, Fig. 148 Fig. 147 Fig. 148
click OK .
Step 10. Click Tools Menu > Sketch Tools > Construction
Geometry.
Step 11. Click all the lines to change lines to construction
lines, Fig. 149. Fig. 149
SolidWorks 08 Body F1 CAR Page 2-27

28. Step 12. Click Line (L) on the Sketch toolbar.
Step 13. Draw line for front of wing as shown in Fig. 150.
Step 14. Click 3 Point Arc (S) in the Arc flyout
Fig. 150
on the Sketch toolbar. 2
3
1
Step 15. Draw 3 Point Arc between Points 1, 2 and 3,
Fig. 151.
Step 16. Draw 3 Point Arc between Points 2, 4 and 5,
Fig. 152. Keep Point 4 away from the horizon-
tal center line. Snap Point 5 to the construction Fig. 151
line at Point 5. Important Point 5 snaps to 2
centerline so it become tangent to the center-
line.
Step 17. Click Smart Dimension (S) on the 4 5
Sketch toolbar.
Fig. 152
Step 18. Dimension the top arc 64, Fig. 153. Dimension
the gap between the horizontal center line and the
bottom arc 1 as shown in Fig. 153.
Step 19. Click Sketch Fillet on the Sketch toolbar.
Fig. 153
Step 20. In the Sketch Fillet Property Manager set:
Radius to 1 , Fig. 154
click the corner shown in
Fig. 155
Radius to 2 , Fig. 156
click the two corners
shown in Fig. 157. To Fig. 154 Fig. 155
Sketch Fillet the bottom fillet,
click the line and the bottom
arc. Click OK to message
deleting geometry relations.
Fig. 156 Fig. 157
SolidWorks 08 Body F1 CAR Page 2-28

29. Step 21. Click Features on the Command Manager toolbar.
Step 22. Click Isometric on the Standard Views toolbar.
Step 23. Click Extruded Boss/Base on the Features toolbar.
Step 24. In the Property Manager set:
under From
Start Condition to Offset
Offset Value to 3
under Direction 1
Depth to 28
click OK , Fig. 158
Step 25. Save. Use Ctrl-S.
Fig. 158 Fig. 159
Y. Create Front Wing Endplate.
Step 1. Rename Extrude1 to FRONT WING
EXTRUDE in the Feature Manager.
To rename, click the feature name and
press F2, Fig. 160.
Step 2. Click the side face of wing and click
Sketch on the Content menu,
Fig. 161.
Fig. 160 Fig. 161 Side face
Step 3. Click Offset Entities on the
Sketch toolbar.
Step 4. In the Offset Entities Property Manager
set:
Distance to 1, Fig. 162.
The yellow offset sketch should be
on the outside of the face, Fig. 163. If
163
it is not, click Reverse. Click OK
.
Fig. 162 Fig. 163
SolidWorks 08 Body F1 CAR Page 2-29

30. Step 5. Click Features on the Command
Manager toolbar.
Step 6. Click Extruded Boss/Base on
the Features toolbar.
Step 7. In the Extrude Property Manager: Fig. 165
under Direction 1
Depth to 2.5
Reverse Direction
The Direction arrow should Fig. 164 Fig. 166
point back towards the body, Fig.
165. If arrow is pointing in wrong direction, click
Reverse Direction , Fig. 164. Click OK
, Fig. 166.
Z. Mirror Front Wing and Endplate.
Step 1. Click Mirror on the Features toolbar.
Step 2. In the Property Manager set:
under Mirror Face/Plane, Fig. 167
expand the Design Tree in the top left
corner of the drawing area
click Right (Plane), Fig. 168
under Features to Mirror
in Design Tree select FRONT WING
EXTRUDE and Extrude 1
Fig. 167 Fig. 168
click OK , Fig. 169.
Fig. 169
SolidWorks 08 Body F1 CAR Page 2-30

31. AA. Create Front Wing Folder.
Step 1. Ctrl click FRONT WING EXTRUDE,
Extrude1 and Mirror4 in the Feature
Manager to select all three. Right click
any of the selected Features and click Add
to New Folder on the menu, Fig. 170.
Step 2. Rename new Folder WING FRONT in
the Feature Manager. To rename, click the
Folder name and press F2, Fig. 171.
BB. Modify Rear Wing Sketch.
Step 1. If necessary, turn on Instant3D on
Fig. 170 Fig. 171
the Features toolbar.
Step 2. Expand the WING FRONT folder.
Hold down Ctrl key and drag
FRONT WING EXTRUDE in the
Feature Manager design tree out and
set on the flat side face of the body
just above the rear axle standout,
Fig. 172.
Step 3. Click Delete in Copy Confirmation
dialog box to delete the external
constraints (dimensions), Fig. 173.
Step 4. Expand Extrude2 (rear wing), click
Sketch17 in the Feature Manager
and click Edit Sketch Plane
from the Content toolbar, Fig. 174.
Fig. 172 Fig. 173
Step 5. In the Sketch Plane Property Manager:
Under Sketch Plane/Face, Fig. 175
Expand the Design Tree in the top left
corner of the drawing area and click Right
(Plane), Fig. 176.
176
Fig. 175
Click OK .
Fig. 174 Fig. 176
SolidWorks 08 Body F1 CAR Page 2-31

32. Step 6. Click Extrude2 (rear wing) in the Feature Manager and click Edit
Sketch on the Content menu, Fig. 177.
Step 7. Click Normal To on the Standard Views toolbar. (Ctrl-8)
Step 8. Click Zoom to Selection (Q) on the View toolbar to zoom
around the read wing sketch.
sketch
Step 9. Click Smart Dimension (S) on the Sketch toolbar.
Fig. 177
Step 10. Add and change Dimensions as shown Fig. 178: Intersection
of centerlines
Add 31 dimension from bottom of body to inter-
section of centerlines
Add 23 dimension from rear of body to intersec-
tion of centerlines
Change length of angled centerline from 20 to 24
(length of sketch)
Change angle of centerline from 18 to 14
Step 11. Click Exit Sketch on the Sketch toolbar.
Fig. 178
CC. Modify Rear Wing Extrude.
Step 1. Use the Rotate View in the View toolbar to rotate
view as shown in Fig. 179.
Step 2. Click the Extrude2 (rear wing) in the Feature Manag-
rear
er and click Edit Feature on the Content menu,
Fig. 178.
Fig. 179
Fig. 180
SolidWorks 08 Body F1 CAR Page 2-32

33. Step 3. In the Property Manager set: Arc face
under From
set Start Condition to Surface/
Face/Plane
set Select a Surface/Face/
Plane: click the outside arc face of
the body at the cartridge hole,
Fig. 182
Fig. 182
under Direction 1
End Condition to Offset
From Surface
set Face/Surface: expand the
Design Tree in the top left corner of
the drawing area click Right (Plane), Fig. 183
Fig. 183 Fig. 181
Depth to 31
click OK , Fig. 184.
DD. Create Rear Wing Folder.
Step 1. Rename Extrude2 to REAR WING EXTRUDE in the
Feature Manager. To rename, click the Folder name and
press F2, Fig. 185. Fig. 184
Step 2. Right click REAR
WING EXTRUDE
and click Add to
New Folder on the
menu, Fig. 186.
Step 3. Rename new Folder
WING REAR in
the Feature Manager.
To rename, click the
Folder name and
press F2, Fig. 187. Fig. 185
Fig. 186
Fig. 187
SolidWorks 08 Body F1 CAR Page 2-33

34. EE. Create Rear Wing Endplate.
Step 1. Click the side face of rear wing and click Sketch
on the Content menu, Fig. 188.
Step 2. Click Offset Entities on the Sketch toolbar.
Side face
Step 3. In the Offset Entities Property
Manager set:
Distance to 1 Fig. 188
The yellow offset sketch
should be on the outside of the
face, Fig. 190. If it is not, click
Reverse. Click OK .
Step 4. Click Features on Fig. 189
the Command Manager toolbar.
Fig. 190
Step 5. Click Extruded Boss/Base
on the Features toolbar.
Step 6. In the Extrude Property Manager:
under Direction 1
Depth to 2.5
Reverse Direction
Fig. 191
Fig. 192
The Direction arrow should point back towards
the body, Fig. 192. If arrow is pointing in wrong direc-
tion, click Reverse Direction , Fig. 191. Click OK
.
Fig. 193
SolidWorks 08 Body F1 CAR Page 2-34

35. FF. Mirror Rear Wing and Endplate.
Step 1. Click Mirror on the Features toolbar.
Step 2. In the Property Manager set:
under Mirror Face/Plane, Fig. 194
expand the Design Tree in the top left
corner of the drawing area
click Right (Plane), Fig. 195
under Features to Mirror
in Design Tree select REAR WING
EXTRUDE and Extrude2
under Options
check Geometry Pattern
click OK , Fig. 196.
Fig. 194
GG. Move Features to Rear Wing Folder.
Step 1. In the Feature Manager, move the
two features into the REAR WING Fig. 195
FOLDER.
To move a feature, drag the feature
over the last feature in the folder.
When the cursor changes to Arrow
release the feature, Fig. 197.
Drag both Extrude2 and Mirror5
into the REAR WING FOLDER,
Fig. 198. Fig. 196
HH. Fillet Edges.
Step 1. Click Fillet on the Features toolbar.
Fig. 197 Fig. 198
Step 2. In the Fillet Property Manager:
Select FilletXpert, Fig. 199.
FilletXpert 199
Set the Radius to 8
Click the edge between rear of side
pod and body on both sides of the
body (hold down middle mouse but-
ton to rotate view), Fig. 200.
Click Apply
R8
Fig. 199 Fig. 200
SolidWorks 08 Body F1 CAR Page 2-35

36. Set the Radius to 12,
Fig. 201
Click the end edges on all 4
corners of side pods, Fig. 202. R 12
Continue and add Fillets: Fig. 202 R 12
Front edge of side pod and
body, Radius 14, Fig. 203.
Fig. 201
Top edge of body and side R 14
pod , Radius 1.5, Fig. 204. Fig. 203
Bottom edge of body and side pod, Radius 1.5, Fig. 205.
Top back edge of cockpit, Radius 2, Fig. 206.
Top front edge of cockpit, Radius 2, Fig. 207.
R 1.5
R2
Fig. 204
Fig. 206
R 1.5
Fig. 205
R2
Fig. 207
SolidWorks 08 Body F1 CAR Page 2-36

37. Bottom edge of cockpit (one side), Radius 2,
Fig. 208.
Bottom edge of cockpit (other side), Radius 2,
Fig. 209.
Both edges of endplate (all 4 endplates),
Radius 1, Fig. 210.
Edge of endplate and wing, Radius 1, Fig. 211.
R2 Fig. 208
Edge of endplate and body, Radius 1, Fig. 212.
1
Click OK when done.
R2
Fig. 209
R1
Fig. 210 R1
R1
R1
Fig. 211 Fig. 212
SolidWorks 08 Body F1 CAR Page 2-37