How to model a Table Tennis Racket with SolidWorks?

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Open a new file using the menu File > New… then select Part. You are now facing a blank screen, ready to start modeling the racket.

The first things to set up here are the blueprints, which will allow us to draw the racket’s shape precisely. They consist here of two images (given below or available in the tutorial’s folder if you download the pdf version), one for the side and the other for the top of the racket. Those images need to be imported in SolidWorks and carefully placed in the scene.

In the FeatureManager on the left-hand side of the screen, select the Top Plane. A tiny set of icons should pop up, click on the first one to create a sketch on the top plane.

Now go to Tools > Sketch Tools > Sketch Picture… and import this file : Top_BP. Complete the properties of the sketch like the left picture below.
Note that you have to unlock aspect ratio in order to edit the X and Y scale independently. You may also add some transparency to the blueprint.
Repeat the same process for the Side_BP picture after exiting the previous sketch. This blueprint needs to be rotated though (right picture below).

The blueprints are now set up!

Now let’s draw the first sketch that will feature the global shape of the racket. We just need to model half of the racket since it is symmetric.

Create a new sketch on the top plane. Start with a straight line. To do so, click on this button:

Draw this vertical line from the origin to the other racket’s end. Then use the Smart Dimension tool to give a precise length to it. Simply click on the line you just drew and write 255 (we work in millimeters here).

Now let’s add a bunch of new lines to this sketch as the following picture illustrates. In order to specify the distance from one horizontal line to the origin, select your line with the Smart Dimension tool then click on the origin.
Most of these lines are dashed. It means that they are for construction purposes. To add this kind of line, expand the line menu by clicking on the little arrow on the right of the line icon.

Add this extra line, defined thanks to two dimensions:

The rest of the shape is not made of straight lines, but rather curves. Find the Spline tool and select it. Start by the end of the line you just added, then click on each construction line’s end. This will constraint the spline in passing through different points. The last point is the origin. Then press Escape to finish.

Granted, it’s curved, but it doesn’t follow the racket’s shape! First of all, select the spline, then with the Shift key pressed, the oblique line. Add a tangency relation:

You probably noticed that the spline contains tangent handles at every point it passes through. Click on the handle at the origin. On the left-hand panel, add a Horizontal relation.
The effect of that manipulation will be to force this handle to remain horizontal. After that, it is up to you to move the handles in order to get the spline as close as possible to the real shape of the racket.
Here is the final sketch:

Exit the sketch. We now want to extrude this sketch to give volume to the racket. On the Features tab, select Extruded Boss/Base Instead of Blind choose Mid Plane. Set the distance to 5.80 mm.

The next few steps will be dedicated to the racket’s handle. We will use the Lofted tool to add volume between two sketches, which is a common way to proceed.

Click on the top surface of the body you just created. You have the possibility to create a sketch on this very flat surface. Once you entered the sketch mode, select the oblique edge again, and Convert Entities

Also draw a vertical construction line of 97 mm from the racket’s end like so:

Furthermore, add a horizontal construction line starting from the lower end of the previous vertical line. Using the Extend Entities tool, click on the oblique line. It should now reach the horizontal line.

Let forget about this sketch a moment. On the vertical surface on the end of the racket’s handle, add this profile. It contains a spline whose right handle is horizontal. It ensures tangency with its symmetric part:

Now, add a new plane by going to Reference Geometry > Plane in the Features tab.

To fill the first reference, click on the Front Plane in the FeatureManager. Then click on the extremity of the oblique line we extended in a previous sketch. This defines a plane.

On this plane, create a new sketch. Draw a line from the center to the oblique line’s extremity. Then add a vertical line of 6.50 mm. Close the profile with a spline. Don’t forget to add a horizontal relation to the handle at the center.

We now have two profiles to create volume. In the Features panel, select Lofted Boss/Base. Then click on the two profiles and uncheck Merge result.

We now want to cut a part of the body we just got in order to give its final shape.

On the right plane, draw this line. It starts at one end of the last body with a 5 mm offset from the top plane and has an angle with this plane of 16 degrees.

In the Features tab, select Extruded Cut once you’re done with the last sketch. Click OK. It basically removed the part above the line!

A table tennis racket has rubber surfaces on its sides. This will be the last part we add to the model. We just need to create such a surface on one side, and symmetrize it.

On the plane defined by the top of the racket's body, create a new sketch. Select the large face of the racket and Convert Entities. It will add the border to the sketch. Draw a horizontal line and trim above using the Trim Entities tool. To do so, hold the mouse button and drag over the lines you want to get rid of.

You should have the rubber surface profile ready. Now extrude it from 3 mm upward. Don’t merge!

Find the Mirror tool. As a symmetry plane, select the Top one. Under Bodies to Mirror select the rubber surface and the handle. Once it’s done, click on the Mirror tool again and select all the bodies and symmetrize them with respect to the side plane. Add colors and textures if you wish to.

Here is the result!