SolidWorks Basics

Launch SolidWorks from any computer in the engineering buildings. You may also install it on your personal Windows machine by following the instructions here.

The basic idea in SolidWorks is to create a 2D shape, add dimensions to it, and then extrude it. In other words you "pull" the 2D shape into a third dimension and give it depth.

Once you have a basic 3D shape then you can add additional 2D shapes on to it and further extrude these.

Alternatively, you can add a 2D shape onto a 3D part and use the 2D shape to create a cut.

There are many more things you can do in SolidWorks, but for the purposes of this tutorial that summarizes everything.

After launching SolidWorks, begin by creating a new part.

Once you have clicked OK to create a new part, be sure to choose metric units of measurement (MMGS) in the bottom right corner of the screen as shown here in green.

Create a center circle by clicking the Circle button within the Sketch tab.

Choose to create your sketch in the Top Plane by hovering your mouse over the correct plane until it highlights orange, then left clicking.

Click the origin of the sketch (small red axes near the center of the screen) to anchor the center of your circle there.

Move your pointer out away from the center of the circle. Create a circle of arbitrary radius by clicking again.

Rotating the scroll wheel of your mouse will zoom in or out on the drawing.

Enter a radius value of 5.0 in the appropriate field in the left window column. Click the green check mark to confirm and exit the circle tool.

This circle will be the outside of the motor shaft extension. Let's view it from the top plane to make it easier to see.

Click the View Orientation button near the top of the screen. A cube will appear allowing you to choose a plane from which to view the sketch.

Hover over the plane you wish to choose. Look at the preview shown at the top right of the screen. Confirm it looks like the example shown here and then click on that plane to orient your sketch properly.

Now add a second, concentric circle inside of the first. This second circle should have a radius of 2.08.

Switch the to Features tab. Click Extruded Boss/Base.

Enter a value of 7.0 for the extrusion height. Click the green check mark in the upper left to accept the value.

Use the View Orientation button again to rotate the newly extruded cylinder so that you are viewing it from the top plane.

Return to the Sketch tab and create a Center Circle which is concentric with your cylinder. Click on one of the faces of the cylinder when prompted for a sketch plane.

Anchor the circle in the center of the cylinder then click the outer edge of the cylinder to make the radius of the new circle identical to that of the cylinder. Confirm that the radius of your new circle is 5 mm.

Click View Orientation and choose to view the cylinder from the top down so that you are viewing the face of the cyclinder where you just added a new circle sketch.

Create another center circle and this time, after clicking the Center Circle button, hover above the existing circle you just drew and move the mouse near the (invisible) vertical axis. A dotted line should appear emerging from the center of the existing circle. This will lock the new circle in line with the existing circle.

Click to anchor the center of the new circle on this line. Create a small circle of arbitrary diameter. In the radius Parameters field in the left column enter a value of 0.2.

Click the green check mark to complete the circle.

Click Smart Dimension. Then click the center of the large circle followed by the center of the small circle. Define this distance to be 33.0 mm.

Within the Sketch tab choose to create a Line. Use your mouse scroll wheel to zoom in on the small circle. Hover over the left edge of the small circle. An orange anchor point should appear. Click this point to anchor the line to be tangent to the left side of the circle.

Now zoom in on the larger circle and hover near the left edge of the this circle. Click the orange anchor point on this circle to terminate the line at the tangent point on the circle's edge. Hit the escape key to stop drawing this line.

Repeat the same process to create an identical line on the right side.

Click the Trim Entities button within the Sketch tab. Use the mouse scroll wheel to zoom in on the small circle.

Click below the small circle and drag the mouse across the bottom of the small circle. The bottom arc of the circle will be trimmed up to the point where it intersects on either side with the tangent lines drawn previously. Release the mouse button. Your sketch should look like the first image here.

Now zoom out and then zoom in again on the bottom circle. This time click above the top edge of the bottom circle and drag the mouse across the circle top edge. The top arc should be deleted up to the point where the tangent lines intersect with it. Release the mouse button.

Finally, zoom in on one side of the large circle. The tangent line has created a cord as it intersects with the circle at two points. Click outside of the large circle and drag the pointer across this outer arc to remove it. Be careful to stop after crossing the arc and do not continue to trim the cord itself.

Repeat this trim on the right side of the large circle as well.

If you do not have a closed path for the pointer arm at this point you should stop and return to the previous step. The extrude will only work properly if you have a closed path. A complete path should appear as a blue outline with a grey shaded interior as shown in the first image here.

If your extrude in this step does not seem to be working check that you definitely removed the two small arcs from the previous step and left the two cords intact.

Within the Features tab choose the Extruded Boss/Base.

Enter a value of 3.1 mm for the height of the extrude.

Rotate the part so that you can see the shaft hole in the bottom face. On the Features tab click the Fillet button.

Enter a radius value of 0.5 mm. Then click the circle for the shaft slot. You should see a preview appear in yellow. Click the green check mark to complete the fillet.

This fillet will gently round the edges of the motor shaft slot to make it easier to attach the arm.

Use the View Orientation button and look at the arm from the bottom side (where you can see the hole you just made). Choose to make a new center circle and place it on the same plane as the arm by clicking on the arm. Do not click on the circular, extruded shaft.

Hover above the existing circles so your new circles shares the same axis as the other circles. This new circle should have a radius of 2.9 mm. Use the Smart Dimension tool to define the distance from center to center of the new circle to the previous circles to 24.3 mm. See the first image here.

Now go to the Features tab and choose to Extrude this circle. In the Direction 1 drop down menu on the left choose "Up To Surface".

Rotate your view (right click somewhere in the white, choose Pan/Zoom/Rotate and select Rotate View) so you can see the top of the arm. Left click on the face of the arm and it should turn pink as in the second image here. Click the green check mark to accept this confirmation.

Make another circle, this time inside of the circle you just made near the end of the motor arm. The circle should have a radius of 1.9 mm.

Click on the Features tab and choose to make an Extruded Cut of type Blind. Enter a value of 2.1 mm. You can rotate your view to make sure the cut is pointing in the correct direction.

We need to have the printer cover the magnet. Return to the Sketch tab and create another center circle. Click on the bottom face of the arm. Anchor the circle in the center of the previous cut and click on the edge of the circular cut you just made.

Confirm that the new circle sketch you just made has a radius of 1.9 mm.

Select Extruded Boss from the Features tab. Choose to make a Blind boss with a depth of 0.4 mm.

The hole you made previously should now be hidden.

The final step is to slightly increase the depth of the very first hole we made. Use the View Orientation button again to view the part from the bottom so you can see the motor shaft hole.

Create another center circle and when prompted to select a plane for the sketch be sure to click inside of the motor shaft hole.

Anchor the circle in the center of the existing circles so that it is concentric with them. Then click on the inner wall of the existing hole to set the radius of the new circle. Confirm the radius is 2.08 mm.

Finally, choose to make an Extruded Cut with depth 0.8.

Save your part as a .sldprt file so that you can modify it later if necessary.

Also save your part as a .STL file. You will need the .STL file to 3D print. Note that you cannot modify an .STL file.

Be sure to click the Options button before saving the .STL file.

Becuase many 3D printer slicing applications operate in metric units, you should confirm that the Unit parameter of your STL file is set to Millimeters.

Click OK and then save your .STL file.

SolidWorks will pop up a window telling you how many triangles your part contains. Click Yes to continue saving.