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 (a sketch), 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 rectangle by clicking the Center rectangle 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 rectangle there.

Move your pointer out away from the center of the rectangle. Create a rectangle of arbitrary size (but roughly skinny and vertical) by clicking again.

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

Click on the Smart Dimension button and then click on the long edge of the rectangle you just drew. Drag the dimension out and click to anchor it. A pop up box will appear and allow you to enter a value. Enter 55.6.

Repeat this process for the narrow dimension and set the value equal to 10.3.

Click the Circle button from the Sketch tab and place a circle near the bottom of the rectangle.

Use the Smart Dimension tool to give the circle a diameter of 3.0 mm and position it 5.3 mm from the left and bottom edges. See the second image.

Clicking on the edge of the circle will allow you to define a diameter.

Clicking on the center of the circle and then an adjacent side will allow you to define the distance from the circle center to that side.

Create a second circle at the top of the rectangle. Give it the same diameter and spacing as the first circle you created.

Since this circle should match the bottom circle you can use the = (equals) sign when dimensioning it, followed by clicking an existing dimension you wish to copy. This creates a pointer in SolidWorks so if the original dimension changes, the pointers will update automatically.

Note the three red Σ (sigma) symbols in front of the top three dimensions in the final image shown here. This indicates these values are pointing to other existing dimensions.

Click on the Sketch fillet button in the Sketch tab. A fillet is a rounding of an interior or exterior corner of a sketch or part.

Click on the top left and bottom left corner points to add them to the list of points to fillet. You should see a fillet preview appear in yellow. Enter a value of 3.3 mm for the fillet radius.

Click the green check mark twice to accept these fillets.

Your sketch should look like the final image shown here.

Click the Extruded Boss/Base button from the Features tab. Your sketch should rotate and a yellow preview of the extrusion will appear.

Enter a depth value of 8.19 mm and then click the green check mark to accept this value and extrude the sketch.

The part should now be shown as a 3D dimensional object.

Return to the Sketch tab and choose to sketch a Corner rectangle. You may need to click the small arrow to the right of the Center rectangle tool to display a drop down menu where you can choose Corner rectangle.

SolidWorks will prompt you to select a plane, planar face, or an edge on which to create a sketch for the entity. Click on the top face of the part.

Anchor the top right corner of the rectangle on the right edge of the face and anchor the bottom left corner of the rectangle some distance below this but not touching the left edge of the face. See the second image.

Use the Smart Dimensions tool to give the rectangle the three dimensions shown in the final image.

Return to the Features tab and choose Extruded Cut.

Change the End condition drop down menu to Through All. This tells SolidWorks to make this cut pass through the entirety of the extrusion, regardless of how deep it is.

Click the green check mark to accept the cut.

There should now be a rectangular cutout in the part. You can use the Rotate View tool to click and drag in order to rotate your part in three dimensions to confirm the cutout went all the way through the extrusion.

The USB C connector is close to the edge of this spacer so we need to remove a small amount of material to compensate for this and allow clearance for the spacer to properly fit inside of the enclosure.

Return to the Sketch tab and create another Corner rectangle. When prompted to choose a face, choose the top of the extrusion like you did in the previous step.

Anchor the top right corner of the rectangle to the top right corner of the extruded part. Anchor the bottom left corner of the rectangle to the bottom edge of this upper portion of the extruded part. See the first image.

Use the Smart Dimensions tool to give the rectangle a width of 1.0 mm.

Return to the Features tab and create an Extruded Cut from this rectangle. Choose an End condition of Through All like you did previously.

The top width should now be slightly more narrow than the bottom width as shown in the final image.

The final step is to add two more fillets. This time we will add fillets directly to existing extrusions as opposed to adding them to a 2D sketch as we did in a previous step.

Within the Features tab click on the Fillet button. Enter a value of 3.0 mm into the Radius box.

Again use the Rotate View tool to rotate the part so you can clearly see the two edges indicated here in red.

Clicking on the indicated edges should provide a preview of the fillets in yellow. Click the green check mark to accept these fillets.

Save your part as a .sldprt file so that you can modify it later if necessary. Give it a meaningful name. If you're working on DA7 for ECEG 201 be sure to indicate that this it the LEFT spacer so you don't confuse it with the additional RIGHT spacer you also need to create.

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