Modelling And Rendering of American Chopper

https://drive.google.com/open?id=1kCd7lQyEA2uoHyaXPv8G6tg3TFgR7S-N

Create a new part

Open a new part with model units set to millimeters.

Go to: File > New > Part

Click on the front plane and draw the sketch as shown in pic

Extrude the drawing as shown using the selected counter option

Again use the selected counter option in Extrude sketch.

Use the fillet option using selection of the face.

Make a new sketch on top plane as shown

Use the revolve command to get the pedal for foot resting.

Go to insert feature and select the dome option

By using the previously drawn sketch of pedal use the contor region extrude to get the other pedal for foot resting. As shown in pic

For aesthetic purpose make a chamfer to the middle and last foot pedal using distance- distance option

as shown below

To create aesthetic rings on extrude pedals again draw the sketch on the front plane. And extrude it from offset distance.

The above extrude is followed by the fillet operation.

Making the linear pattern of the extrudes we get the desired structure.

Fillet the remaining edge of pedal and save the part.

Now go to appearances and give it chrome finish. Save the part as a part name Pedal.

In this tutorial you will learn the following features:

1. Draw a 2d sketch
2. Revolved Surface
3. Surface Trim
4. Thicken
5. Extruded Cut
6. Fillet

Create a new part

Go to: File > New > Part

• Change the names of the planes
• Double click on the Front Plane in the feature tree.
• Change the name to: VERTICAL PLANE FRONT FENDER
• Double click on the Top Plane in the feature tree.
• Change the name to: CENTERPLANE FRONT FENDER
• Double click on the Right Plane in the feature tree.
• Change the name to: MIDPLANE FRONT FENDER
• Create a 2D sketch
• Sketch by on VERTICAL PLANE FRONT FENDER clicking on the 2D Sketch icon.
• Draw a 3 Point Arc

Go to Tools > Sketch Entities > 3 Point Arc or click on the

• 3 Point Arc icon.
• Select the 3 point arc
  • Click to create the first endpoint.
  • Click again to create the second endpoint.
  • Click for the third time to create the radius of the arc.
• Make the endpoints of the arc parallel to each other
• Select the first endpoint of the arc. Hold down the Control key on your keyboard and select the second endpoint of the spline. Select the Horizontal relation in the Add Relations toolbar.
• Change the dimensions of the arc as shown in the picture by clicking at the dimension button.
• Draw a horizontal centerline starting at the origin as shown in the picture.

• Create a Revolved Surface
• Go to: Insert > Surface > Revolve or click on the Revolved Surface icon.
• Select the horizontal centerline as the Axis of Revolution.
• Select the One-Direction option.
• Change the Angle into 360 degrees.
• Click OK.

• Create a 2D sketch
• Select the MIDPLANE FRONT FENDER and create a sketch by clicking on the 2D Sketch icon.
• Draw the two lines as shown in the picture.

Go to Tools > Sketch Entities > Line or click on the Line icon.

Draw the sketch as shown in pic and make it fully contrained.

Go to: Insert > Feature> split icon.

Select the sketch drawn and use the tool to remove the unwanted part

Select the purple piece to keep. Click OK.

Do the same procedure for another side of fender.

Change the color of the part

Click on the Front Fender model.

Click on the appearances button.

Click on the Body option.

Change the color to orange. Click OK.

Select the CENTERPLANE FRONT FENDER and create a new sketch

Draw a vertical construction line starting at the origin.

Draw a spline and add the dimensions.

Mirror this spline about the vertical construction line in the middle of the sketch.

Create a Surface Fillet

Go to: Insert > Features > Fillet/Round or click on the Fillet icon.

Click on the green surface as shown in the picture.

Change the Radius into 6 mm. Click OK. Save as Front_Fender.SLDPRT file.

Create a new part

Open a new part with model units set to millimeters.

Go to: File > New > Part

Click on the front plane and draw the sketch as shown in pic

Now use the revolve command to make the rim part of the front wheel. As show in picture

Click on right plane and click on sketch, for making the alloys of the wheel rim. Use the splines to get perfect shape of the alloys. Adjust the handle and weights of the spline as given in pic.

Use boss/base extrude command with mid plane extrude type. i.e. both side of mid plane.

Now use drawing as shown in pic. Use offset command to draw the alloys of the wheel.

Cut extrude command with selected contour option. Select the green zone for alloys on the both side of mid plane.

Make the connection between different alloys with some connection part.

Using the boss base extrude connect the alloys to each other. Use from sketch plane to vertex and chose the point on alloy.

For giving the shape to connection, click on the front plane and draw the pattern which will cut the material from connecting alloys.

Now use the cut revolves command to remove the unwanted material from alloy wheel. As given in the pic. Select the part from which we want to remove the material (select contour option).

Now make the pattern of fully created alloys as shown in pic

Combine the all separate alloys together using combine feature. Go to insert- feature- combine.

Select the bodies to combine click on combine. It will merge the bodies and form one part.

Click on right plane- make new sketch. Draw a circle to make disc of break. Extrude the drawing as shown in pic. Select the option Offset from sketch surface and give the extrude value.

Now select the surface of disc and use it as a plane, click on sketch. We are now going to make the drawing for hole in disc brake.

With the use of extrude cut create the holes in the disc plate. Use the selected countor option.

Repeat the cut extrude to make a circular pattern.

By using cut extrude make the hub for front wheel.

For making calipers to disc draw the sketch on disc as shown in pic

Extrude the same sketch in both sides of disc to make it caliper of disc brake.

Give some chamfers and fillet to give it aesthetic look.

To model the tyre on the wheel rim, click on the front plane to make the sketch.

Revolve the same sketch around the x axis. It will create the tire like shape. Use

combine feature to add the all parts, to make all parts as united.

Now it is essential to make design pattern on the tire surface to make better grip on the ground. We are going to use extrude cut and circular pattern of the same. Click on front plane and make the sketch as shown

We gonna use cut extrude to make the slots on tire surface with the help of Feature scope option. Select the tire for feature scope option. The cut extrude will only affect the tire surface.

Add some fillets and make the circular pattern of same features created above to get the complete tire design.

Now save the part as Front wheel.

Do the same process for Rear wheel.

Features which are going to be used:

1. Draw a 2d sketch
2. Extrude
3. Extruded Cut
4. Loft
5. Dome
6. Fillet

Create a new part

Go to: File > New > Part

• Change the name of the Right Plane. Click three times slowly it will change the name of file in feature tree.
• Change the name to: MIDPLANE KICKSTAND
• Select the Front Plane and create a sketch by clicking on the 2D sketch icon
• Draw an ellipse
• Go to: Tools > Sketch Entities > Ellipse.
• Click on the origin. The origin must be the middle of the ellipse. Enter the dimensions of the ellipse as shown in the picture.

• Click at the Sketch button in the upper right corner to close the 2D Sketch
• Draw a Spline and connect it to the Ellipse of Sketch 1

Go to: Tools > Sketch Entities > Spline or click at the Spline icon.

Draw a spline without any midpoints as shown in the picture.

• Select the right endpoint of the spline, hold down the Control key and select the top point of Sketch 1 as shown in the picture.
• Click at the Coincident icon in the Add Relations box. Click OK.
• Enter the dimensions of the spline as shown in the picture.
• Change the curve of the Spline
• Click on the right endpoint of the spline, the grey arrows of the Spline will appear.
• Select the Horizontal relation in the Spline menu bar at the left side.
• The endpoint of the spline is now fully horizontal.
• You can change the shape of the spline by dragging the tangency arrow.
• Decrease the size of the arrow to create the global curve as shown in the picture.
• Click on the Sketch button in the upper right corner to close the 2D Sketch.
• Create a new plane

Go to: Insert > Reference Geometry > Plane

• Select the left endpoint of the spline of Sketch2 as First Reference.
• The new plane appears in yellow.
• Select the Spline as second reference.
• The direction of the new plane is perpendicular to the spline.
• Click OK.
• Select the new Plane1 and create a new sketch
• Select the “Normal To” option in the View Orientation bar.

Draw an ellipse

Go to: Tools > Sketch Entities > Ellipse

Draw an ellipse as shown in the picture.

• Enter the dimensions of the ellipse as shown in the picture.
• Select the upper point of the ellipse, hold down the Control key and select the Origin as shown in the
• Click on the Coincident icon in the Add Relations box
• Click OK
• Select the upper point of the ellipse, hold down the Control key and select the lower point of the ellipse.
• Click on the Vertical icon in the Add Relations box to fix the sketch (the sketch will turn to black)

Create a Solid Loft

Go to: Insert > Boss/Base > Loft or click on the Loft icon.

• Click in the Profiles Box: Select Sketch1 and Sketch3.
• Guide curves influence: To Next Guide.
• Click in the Guide Curves Box: Select the purple Sketch2.
• Click OK.

Create a dome

Go to: Insert > Feature > Dome or click on the Dome icon.

• Select the blue face of the loft as shown in the picture.
• Change the Distance into 13 mm.
• Select the “Elliptical dome” and the “Show preview” options.

Click OK.

• Create another dome to the other side of the loft
• Select the blue surface of the loft as shown in the picture.
• Change the Distance to 5 mm.
• Select the “Elliptical dome” and the “Show preview” options.

Click OK.

• Create a 2D sketch
• Select the MIDPLANE KICKSTAND and create another sketch by clicking on the 2D Sketch icon.
• Draw a Centre Rectangle
• Go to Tools > Sketch Entities > Centre Rectangle or click on the Centre Rectangle icon
• Start the rectangle at the origin as shown in the picture.
• Change the dimensions of the rectangle by clicking on the dimension button.

• Create an Extruded Cut

Go to: Insert > Cut > Extrude or click at the Cut Extrude icon.

• Direction 1: Mid Plane.
• Change into: 100 mm. Click OK.
• Create a new sketch on Plane1
• Select Plane1 and create another sketch by clicking on the 2D Sketch icon.
• Select the “Normal To” option in the View Orientation bar.
• Rotate the model 180 degrees with the right or left arrow buttons on your keyboard.
• Draw a Center Rectangle

Go to Tools > Sketch Entities > Centre Rectangle or click at the Centre Rectangle icon

• Draw a centerline from the centre of the rectangle to the Origin
• Change the dimensions of the rectangle and centerline by clicking at the dimension button.
• Create an Extruded Cut

Go to: Insert > Cut > Extrude or click at the Cut Extrude icon.

• Direction 1: Mid Plane.
• Change into: 184 mm.
• Click OK.
• Create a circle on the Top Plane
• Select the Top Plane and create another sketch by clicking on the 2D Sketch icon.

Go to Tools > Sketch Entities > Circle or click on the Circle icon.

• Start the circle at the origin as shown in the picture
• Change the dimensions of the circle by clicking on the dimension button.
• Create an Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click on the Extrude icon.

• Change the Blind Direction into Mid Plane.
• Change into 8 mm.
• Click OK.
• Create two Fillets

Go to: Insert > Features > Fillet/Round or click on the Fillet icon.

• Click on the two green edges as shown in the picture:
• Change the Radius into 2 mm.
• Click OK.
• Create a face Fillet

Go to: Insert > Features > Fillet/Round or click at the Fillet icon.

• Change the Radius into 0.5 mm.

• Click OK.
• Change the color of the part
• Click on the Kickstand model.
• Click on the appearances button.
• Click on the Body option.
• Change the color to light grey.
• Click OK.
• Save the Kickstand.SLDPRT file.

Create a new part

Go to: File > New > Part

• Change the names of the planes
• Double click on the Front Plane in the feature tree.
• Change the name to: MID PLANE OIL TANK
• Create a 2D sketch
• Sketch by on TOP PLANE clicking on the 2D Sketch icon.

Go to: Features tab > Extrude

• Draw the sketch on mid plane oil tank
• Draw the sketch by using line as shown in pic. Use the spline for getting good curvature. Give the dimensions as shown in pic.
• After completing the constrained sketch go to Boss extrude in features tab.

Now use the combined tool

Go to Insert> Feature> Combine

Select the two different solid to combine together.

• Use the fillet command to fillet the sharp edges.
• Now use the Shell command to make the tank hollow from inside.

Go to> Insert> feature> Shell

Select the faces to remove and give the thickness to the part. As shown in pic below

Procedure is as same as Front Fender

7. Draw a 2d sketch
8. Revolved Surface
9. Surface Trim
10. Thicken
11. Extruded Cut
12. Fillet

Create a new part

Go to: File > New > Part

• Change the names of the planes
• Double click on the Front Plane in the feature tree.
• Change the name to: VERTICAL PLANE FRONT FENDER
• Double click on the Top Plane in the feature tree.
• Change the name to: CENTERPLANE FRONT FENDER
• Double click on the Right Plane in the feature tree.
• Change the name to: MIDPLANE FRONT FENDER
• Create a 2D sketch
• Sketch by on VERTICAL PLANE FRONT FENDER clicking on the 2D Sketch icon.
• Draw a 3 Point Arc

Go to Tools > Sketch Entities > 3 Point Arc or click on the

• 3 Point Arc icon.
• Select the 3 point arc
  • Click to create the first endpoint.
  • Click again to create the second endpoint.
  • Click for the third time to create the radius of the arc.
• Make the endpoints of the arc parallel to each other
• Select the first endpoint of the arc. Hold down the Control key on your keyboard and select the second endpoint of the spline. Select the Horizontal relation in the Add Relations toolbar.
• Change the dimensions of the arc as shown in the picture by clicking at the dimension button.
• Draw a horizontal centerline starting at the origin as shown in the picture.

• Create a Revolved Surface
• Go to: Insert > Surface > Revolve or click on the Revolved Surface icon.
• Select the horizontal centerline as the Axis of Revolution.
• Select the One-Direction option.
• Change the Angle into 360 degrees.
• Click OK.

• Create a 2D sketch
• Select the MIDPLANE FRONT FENDER and create a sketch by clicking on the 2D Sketch icon.
• Draw the two lines as shown in the picture.

Go to Tools > Sketch Entities > Line or click on the Line icon.

Draw the sketch as shown in pic and make it fully contrained.

Go to: Insert > Feature> split icon.

Select the sketch drawn and use the tool to remove the unwanted part

• Select the purple piece to keep. Click OK.
• Do the same procedure for another side of fender.
• Change the color of the part
• Click on the Front Fender model.
• Click on the appearances button.
• Click on the Body option.
• Change the color to orange. Click OK.
• Select the CENTERPLANE FRONT FENDER and create a new sketch
• Draw a vertical construction line starting at the origin.
• Draw a spline and add the dimensions.
• Mirror this spline about the vertical construction line in the middle of the sketch.

Create a Surface Fillet

Go to: Insert > Features > Fillet/Round or click on the Fillet icon.

Click on the green surface as shown in the picture.

Change the Radius into 6 mm.

Click OK.

Save as Front_Fender.SLDPRT file.

How to model a Transmission Belt in SolidWorks

1. Draw a 2d sketch
   1. Start with new file click on New Part.
   2. Select the required plane in this case Front plane.
   3. Draw the two circles with given dimension, anywhere in front plane.
   4. Click on center of one of circle holding ctrl key on key board and click on another center of circle giving them Horizontal relation, which will constrain the drawing w.r.t. origin.
   5. Use trim entities option- click on Power trim option and remove the unwanted sketch entities.
   6. After completing constrained (fully defined) sketch, it will turn into black from blue then exit the sketch.

2. Extrude 2D drawn sketch

1. Click on features tab. Select the previously drawn sketch and click on extrude.
2. Select the extrude from Sketch Plane i.e. Front plane. And in one direction. Give the required extrude dimension here it is 80mm.
3. Give the thickness to the extrude feature 3.5mm and say ok.

3. Appearance
4. Click on the appearance tab and give the material according to the requirement. Here it is transmission belt so I have given the rubber material and its appearance.

4. Save

Save the part as Transmission Belt.

Assembling every part in solidworks is easy. Go to new and select the assembly.

Now browse for the part on which maximum numbers of parts are going to fit on it. Or select the main/big part.

In this case select the Chasis on which all parts are going to be fixed.

Now on chasis mount the engine of the chopper. Mate the planes accordingly. Rest the engine on the chassis so that it will be fixed on the chassis.

Now for the holes at the bottom, browse for the pedal from part. Make it concentric with the hole. Arrange the plane accordingly. Make the pedal fully contrained.

Now insert the kickstand at the position. Use the stand hole on chassis and match the outer portion of kickstand.

Fit the transmission belt on the engine rotor. Use width to fit relation to fit the belt on the rotors of engine.

Place the oil tank on the engine itself; just arrange the planes to mate and use bottom of tank and surface of engine coincident.

Arrange the rear wheel of chopper. Make the relation with the chassis. So that it will constrain the motion.

Arrange the all other parts according to position.

Finally you will get the fully assembled American chopper.