Download the annotated text guide with pictures or follow along with the video below.

• Start your design using the F1 Model Block and the Virtual Cargo body template. (F1inSchools_Blank-Cargo.par)
  • Uncheck the feature in PathFinder to hide the Virtual Cargo body.
• Add a new body to create actual Car Body design.
  • Add Part body and name it “Car Body”.
• Click on the Project to Sketch command.
  • Using the orientation cube in the lower right corner, click on the Right view.
  • Press F3 to lock to the Right plane.
  • Select the bottom edge of the F1 blank to project to the plane.
• Draw a 10 mm diameter circle tangent to the left edge of the F1 blank and 12 mm from the bottom edge.
• Add angled lines tangent to the circle on the top and bottom as shown.
  • Add a vertical alignment between their endpoints.
• Sketch 2 more lines approximately as shown.
• Add dimensions using the Smart dimensioning tools to get the desired shape and size.
• Press CTL+I to orient to an isometric view.
• Select the closed regions formed by the sketches and begin to drag into 3D.
  • Press the Shift key to toggle on symmetry to drag in both directions.
  • Drag the 3D body 64 mm.
• Select the circle command and use F3 to lock to the end face of the stock body with the hole.
  • Sketch a 32 mm diameter circle concentric with the hole in the stock body (This is also the origin of the base coordinate system).
• Sketch 2 lines tangent to circle and extending vertically to silhouette edge of the end cylindrical face of the first extrusion.
  • Touch the edge arc of the extrusion to align to the silhouette point.
  • Close the sketch.
• Uncheck the F1 blank feature to hide the stock body
• Select both regions formed by the sketches extrude into the body 70 mm.
  • Use the Shift key to toggle symmetry off and the Space Bar to toggle Adding material.
• Turn on the display of the F1 Blank feature.
• Using the Project to Sketch command again, lock to the end face of the F1 Blank.
  • Select the circular edge of the bore in the F1 blank.
  • Select 3 edge of the slot.
• Use the region of the circle to cut a hole in the Car Body that is 52 mm deep.
• Hide the stock body and rotate the model so you are looking at the bottom of the part.
• Select the extrude command and change the selection option to chain in the command bar.
  • Select one line from the slot profile to chain will select all 3 lines.
  • Right click to accept the selection and then move your cursor to point the arrow to the inside of the U-shape as the side of the open profile to remove and click to set this option.
  • Press the spacebar to toggle removing material and drag the profile completely through the part and finish the cutout.
• Next we want to create a lofted extrude to add aerodynamic features to the car.
  • Select the Point command and lock to the top face of the car body using F3.
  • Touch the right edge of the locked face to find its midpoint to align with and click to create a point on the face.
  • Add a Smart dimension to the Point and make it 10 mm from the edge.
• Select the Loft command.
  • Select Face option in dropdown menu to select front face of cartridge housing.

HINT: be sure the point appears at the end of the tangent line as indicated by the red arrow.

• Change the selection option to Point from dropdown and select the sketch point.
• Click the Preview in the command bar or right mouse click to preview the Loft.
• From the tangency control drop down, select Tangent Continuous.
  • Set to 1.500
• Click Finish.
• Rotate the model to see the bottom face (slot side).
• Select the Rectangle by Center command and lock to the bottom face of the car body using F3.
  • Select “Bottom” on the view orientation cube in the lower right.
• Sketch a rectangle centered on the edge of the body.
• Add dimensions to size and locate the rectangle.
• Mirror the rectangle about the Y axis.
• Use the regions created by the rectangles to cut wheel well slots in the car body.
• Select the wheel well cutout features from the PathFinder (last Cutout feature).
  • In the command bar select the option to move with copy.
  • Select the arrow on the steering wheel to initiate a synchronous copy/move.
  • Copy the cutout 100 mm to the front of the car body.
• Select the front face of the last cutout and select the arrow to start a synchronous edit.
  • NOTE: symmetry automatically selects the face on the opposite side.
  • Drag through the end of the part.
• Add 100 mm radius rounds on the top and bottom edges between the top face of the body and the rear angled faces.
  • Add to both sides of the car
• Select the Circle command and lock to the inside face of the rear wheel well.
  • Select the Right orientation using the view cube.
  • Sketch two 5 mm diameter circles approximately as shown; be sure that they are in horizontally aligned.
  • Add concentric 26 mm circles to represent the size of the wheels and set these 2 circles to construction.
• Add dimensions shown to fine tune their locations.
• Add holes for wheels using extrude cut
  • Using the regions created by the inner circles, drag holes completely through the part.
• Right click in the graphics window to bring up the shortcut menu and select the option to Transitioned to Ordered at the bottom of the menu.
• Add rounds to the following area:
  • Add 3 mm rounds along cylindrical cockpit.
  • Add 2 mm rounds to the front 4 corners of the fuel tank area and then to the top and bottom edges.
  • Add 1 mm rounds to the rear wheel wells and back of the cockpit housing.
• Click on the check box next to Virtual Cargo in the Pathfinder to bring the part into view.
  • Select the virtual cargo by clicking on the part or selecting from the pathfinder.
  • Click on the bottom arrow to drag the part downward.
  • Drag the part into the car body such that it is completely inside.
  • Check by switching the view to wired view under the view tab.
• Return to the normal view and uncheck the virtual cargo from the Pathfinder.
• From the view tab, use Part Painter feature to paint the cockpit are to your the desired color’.
• Save part with a new name to avoid overwriting original template.

Download the annotated text guide with pictures or follow along with the video below.

• Start your front wing design by using the previously made F1 Body design part. (Car_Body.par)
• Create a new assembly.
  • Select “Assembly of Active Model” option
  • Save the new F1 assembly ex. (My_F1_Car_Assembly.asm)
• Create new part in place.
  • Select “Create Part in Place”.
  • Select OK when dialogue box comes up.
  • Select Polyurethane for material in dropdown menu.
  • Click Green checkmark button.
  • Save the part file ex. (front_wing.par)
• Click on the Project to Sketch command.
  • Using the orientation cube in the lower right corner, click on the Right view.
  • Press F3 to lock to the Right plane.
  • Select both front edge and bottom edge of model.
• Click on the offset button to create offset line parallel to front edge.
  • Change the distance to 3 mm.
• Create a line perpendicular to
  both front edge and offset line.
• Select the trim button to trim
  the remaining line on the sketch.
• Create angle dimension for the sketch.
  • Set 40° angle between offset line and bottom edge.
  • Lock the angle using the locking button.
• Set vertical distance for the wing using smart dimension.
  • Select horizontal side and angled side to create the dimensions.
  • Set measurement to 20 mm.
• Click on the region inside the sketch and extrude using the arrow which pops up.
  • Press shift to toggle symmetry.
  • Set extrude to 80 mm.
• Click on the line command.
  • Hover the cursor over the end face of the previous extrusion until it highlights.
  • Press F3 to lock the plane.
  • Press CTRL+H to orient the view to
    the plane
• Sketch 3 lines similar to the ones
  shown in picture.
• Create fourth line by offsetting the edge with the wing.
  • Use the Project to Sketch button.
  • Select “Project with offset” option and click OK.
  • Select the edge with the wing and offset by 3 mm.
• Use the Trim Corner command to connect the ends of the sketch lines.
  • Click and drag around the corners to remove extra lines or to extend the corners.
• Using Smart Dimension, add dimension
  to the sketch as shown.
• Select both sketch and outer face of wing to extrude.
  • Select the add options in extrude toolbar.
  • Deselect the symmetric option.
  • Extrude 3 mm into the wing.
• Add rounds to wing’s outer body.
  • Select the edge/corner option from the dropdown menu.
  • Select the two acute edges and set their radius to 1 mm.
  • Select the two obtuse edges and set their radius to 5 mm.

• Use the Face option from dropdown menu to round entire end face.
  • Set radius to 1 mm.
• Use mirror option to copy the outer body on one side of the wing to the other side.
  • Select the entire outer feature by clicking and dragging
    a box around the geometry.
  • Select the Mirror button.
  • Select the right plane using the coordinate system.
• Use the Part Painter on the View tab to color
  the wing support structure Black (dull).
  • Click and drag around the structure.
• Create a projection of the slot in the bottom of the car body.
  • Select project to sketch button.
  • Lock to the XZ plane from the coordinate system.
  • Select the 3 edges of the slot in the front of the car body.
• Add slot in the wing by removing material.
  • Click on the Extrude command.
  • Select chain option from dropdown menu.
  • Select the 3 projected edges on the XZ plane with one click.
  • Select the cut option from dropdown menu.
  • Point the arrow to the inside of the slot shape and click.
  • Drag the cut through the front wing.
• Isolate the wing by hiding the rest of the body by pressing CTL+Q.
• Add a “Rectangle by center” to the top thickness face of wing.
  • Define the center of the rectangle to be on the
    midpoint of the edge of the face.
  • Add dimensions to the drawing as shown.
• Click on the region defined by the sketch and select arrow to extrude 10 mm towards the slot.

• Show the Car Body (CTRL+Q) and notice how the wing interferes with the body.
  • Click on the Subtract command on the Features tab.
    • Select the Body as the target for the subtraction.
    • Select the Front Wing as the tool body.
• In place activate into the car body by clicking the Edit in place button
  after selecting the body, and notice the new pockets in the car body
  for the Front Wing.
• Select the bottom face of the Front wing key slot.
  • Remove the material by dragging the face downward through the bottom slot.
• Add Rounds to the edge of the extrusion.
  • Use the edge/corner option from dropdown menu.
  • Add 0.5 mm rounds to the edges.
• Add round to the front of the car body.
  • Use the chain option from dropdown menu.
  • Type in radius of 1 mm.
  • Select the edge of the front face of the car body.
• Close and return to the assembly.
• Isolate the Front Wing by selecting it and clicking on the Edit in place icon.
• Click the Round command and select the top edges of the feature.
  • Add 1 mm rounds.
• Click arrow underneath round button for more options.
  • Select Chamfer Equal Setbacks option.
  • Select the edge of the extrusion.
  • Set the setback distance to 0.5mm.
• Finally round the bottom front edge of the wing using the round button.
  • Set round to 1mm.
• Select Close and Return to go back to the top level assembly.
• Save the assembly.
• You have now completed the Front Wing of the F1 Car.

Download the annotated text guide with pictures or follow along with the video below.

• Start your rear wing design by using the previously made F1 Body design assembly. (My_F1_Car_Assembly.asm)
• Create new part in place.
  • Select “Create Part in Place”
  • Select OK when dialogue box comes up.
  • Select Polyurethane for material in dropdown menu.
  • Click on the Green checkmark button.
  • Save the part file ex. (rear_wing.par)
• Orient the model in order to sketch on the correct plane.
  • Using the orientation cube in the lower right corner, click on the Right view.
  • Press F3 to lock to the Right plane.
• Click on the arc button and select “Arc by 3 Points”.

• Draw an arc using 3 points above the car body.
  • This is an estimation and correct dimension will be applied later.

• Using the line sketch feature, draw a line starting from the centerline of the rear wheel axle upwards.
• Click on the connect button in Relate section to align the arc center to the vertical line.
• Using the same connect button, connect the arc and the centerline to remove the remaining arc segments.
• Draw another line from the arc centerline to the other end of the arc.
• Click on the construction button and select both straight lines.
• Using the smart dimensions, define the radius of the arc 70mm.
• Define the angle of the arc 25 degrees.
• To define the thickness of rear wing:
  • Offset the arc by clicking on the offset button and selecting the arc.
  • Offset the arc to the inside 3 mm.
• Sketch an angled line from the lower endpoint of the arc
  • Line should be at a 135° angle as shown.
  • Press the tab key to enter the angle dimensions instead of length.
• Sketch a circle on the trailing edge to create the back end of the wing.
  • Select the tangent circle option from the dropdown menu.
  • Place the circle between the two arcs.
  • Apply a third tangent relationship between the arc and the angled line as shown.
• Taking advantage of the synchronous technology, click and drag a box around the sketch to select the enclosed shape.
• Extrude the enclosed shape 80 mm.
  • Press shift to toggle symmetry.

• Since we no longer need the sketch, we can delete the sketch in the pathfinder.

• Sketch 3 lines on the center plane to create the mounting structure for the rear wing.
  • Using the smart dimensions, add a few dimensions to the sketch.
• Use the extrude feature to create a solid extrusion.
  • Extrude the structure 20 mm symmetrically.
  • Make sure to select chain option from the dropdown menu.

• Use the subtract feature to subtract the wing from the car body.
• Add rounds to the model to make it aesthetically pleasing.
  • Round the 4 corners on the support structure.

• Sketch a rectangle by center on the back side of the wing.
  • Dimension the rectangle 3 mm wide and 6 mm height.
• Extrude the lower region of the rectangle.
  • Extrude 22 mm towards the leading edge of the wing.
• Using the Pathfinder, delete the rectangle sketch.
• Use the coincident plane feature to create a plane coincident to the side of the mounting structure.
  • Using the steering wheel, translate the plane so that it is coincident to the end face of the wing.
• Use the new sketch plane to create a sketch for the support structure at the end of the wing.
  • Use smart dimensions to add a few measurements to the sketch.

• Select the sketch and the wing arc to extrude 3mm towards the center plane.

• Add rounds to the 4 corners of the structure for aesthetic purposes.
  • Select face round option in the drop down menu to add round to the entire face of the support structure.
• Click and drag a box around the entire support structure to select it.
  • Mirror the entire structure across the center plane using the mirror feature command.
• Use part painter feature to paint the two end structures of the wing.
  • Paint the structures Black (dull).
• Click on the “Close and Return” button to close and return to the top level assembly.
• Use the subtract feature to subtract the rear wing body from the car body to remove the interference
• Uncheck the box next to rear wing part in the pathfinder so that you can see the slot in the car body.
• Click on the car body and select edit in place
  • Extend the resulting slot by dragging the end face beyond the edge of the part
  • Also drag the front end of the slot an extra 2 mm.
• Add rounds to the corners of the slot using the Round feature.
  • Specify a 0.5 mm radius for these
• Click on “Close and return” button to exit and return to the assembly.
• Check the box next to rear wing part in pathfinder to see the entire assembly.
• Select the rear wing and click Edit in Place option to work with only the wing.
  • Add chamfers to the bottom edge of the key.
  • Select “Chamfer Equal Setbacks” from the dropdown menu.
• Add 2 mm rounds to the bottom of the wing.
  • Make sure to round all four sides of the wing as shown in the picture below.
• Click on Close and Return button.
• Save the assembly to save the changes to the parts.
• Now you have completed the rear wing of the F1 Car.

Download the annotated text guide with pictures or follow along with the video below.

• Start by opening the previously made F1 Body design assembly. (My_F1_Car_Assembly.asm)
• Expand the Parts Library from the fly-out menus.
• Navigate to the folder ..\F1_in_Schools\_Library
• Click and drag the axle from the library into working space.
• Align the centerline of the axle to the rear hole in the car body.
• For cylindrical object, automatic axial alignment is created.
• For the second relationship, select the center plane relationship from the drop down menu.
• In the Quick bar, be sure the option is set to Double.
• Select the two end center points of the axle and then two side faces of the car body.
• Press esc to exit the Assemble command.
• Drag another axle into the working space.
• You can drag the axle from Parts Library or click and drag from Pathfinder to make another copy of the axle.
• For aligning the front axle, repeat the same steps used for back axle.
• Click and drag the Wheel Spacer from the Parts Library to create space between the wheels and the car body.
• Align the centerline of the spacer with the rear axle centerline.
• Automatic centerline relationship is created by simply clicking on the rear axle.
• Click on the car body face to create second relationship as shown in the picture.
• Press esc to exit the assembly.
• Click and drag a Wheel Assembly from the Parts Library.
• For the first relationship, mate the Wheel to the outer edge face of the spacer.
• For the second relationship, align using the centerline of the spacer.
• Repeat the previous two steps to assemble the remaining three spacers and wheels.
• Click and drag a Pin from the Parts Library.
• For first relationship, align using the centerline of pin and the hole in the axle
• For second relationship, select the axle face adjacent to the wheel.
• Press esc to exit.
• Repeat the previous step to assemble the remaining three pins.
• Click and drag the CO2 cartridge from the Parts Library.
• For first relationship, align using the centerline of CO2 cartridge and the centerline of the bore hole in the back of the car body.
• For second relationship, select the tangent relationship from the drop down menu.
• Select the spherical end of the cartridge and the inside of the bore hole.
• Press esc to exit.
• Click and drag the eye screw from the part library.
  • For first relationship, select the mate relationship from the dropdown menu.
  • Mate flat face of the eye screw with the face of the slot.
• For second relationship, select the center plane relationship from the drop down menu.
  • Set the option to Single.
• Select the centerline of the eye screw and two lateral faces of the slots to align.
• Press esc to exit.
• Click on the eye screw to select it.
  • Orient the model by clicking the front side of the cube in lower right side of the screen.
• Use the steering wheel to bury to the screw into the car body.
  • Lower the screw into the body around 1.8 mm.
  • Click on the delete button in dialogue box which appears.
• Using the steering wheel to move the eye screw behind the rear axle.
• Select the Move -Copy option to create a copy and drag the eye screw towards the front of the car.
  • Around 150 mm from the back eye screw
• This completes the car assembly.

Download the annotated text guide with pictures or follow along with the video below.

• Start by opening the previously made F1 Body design assembly. (My_F1_Car_Assembly.asm)
• To enter the face priority selection mode while working in the assembly:
  • Press and hold the Ctrl key, then press the spacebar to enter editing mode.
• Select the lateral face at the front of the car as indicated in the picture.
  • Click and drag the steering wheel to the vertical edge to pivot the face.
  • Click on the torus of the steering wheel to initiate rotation.
  • Rotate the face -30 degrees.
• Relocate the steering wheel to the top edge of the same face.
  • Click the middle of the steering wheel and drag to desired location.
  • Rotate the face -25 degrees.
• Notice the changes made to one side is applied to the other side automatically.
• Move the steering wheel to lateral edge of the side of the car.
  • Click and drag the arrow along the same axis to shorten the length as shown in the picture.
  • Change the length to 15mm.
• Click on the back face of the same structure.
  • Click and drag the steering wheel to the vertical edge.
  • Rotate the face 8 degrees to add more clearance for the wheel.
• Click and drag the steering wheel to the top edge of the face.
  • Rotate the face 25 degrees.
• Select the face behind the rear wheel.
  • Click and drag the steering wheel to the vertical edge of the face.
  • Rotate the face -8 degrees.
• Move the steering wheel to the bottom edge of the face.
  • Rotate the face 10 degrees.
• Select lateral face at the end of the car body.
  • Click and drag the steering wheel to the vertical edge of the face.
  • Rotate the face -30 degrees.
  • Remember to uncheck coplanar option from the design intent box.
• Orient the model to a right side view by clicking the view box at the bottom right corner of the screen.
• Click and drag a box around the front of the car to select the front include the front wing.
  • Move the Steering wheel above the car.
  • Click the arrow on the steering wheel to shorten the length of the car.
  • Shorten the length to 12mm.
• Select the complete front of the car including the front wheel.
  • Click and drag a box around the desired features to select.
  • Shorten the length additional 12mm.
• You have now completed the F1 Car assembly.
  • KeyShot can be used to generate photo-realistic renderings of your car.