Introduction to SolidWorks Part 1 – Shaping and Joining

Firstly we are going to create a hollow half sphere with mounting holes (as shown). This will be done to introduce you to Shelling, Extruding, Filleting and Extrusion Cutting.

Making a part By Starting a New file in SolidWorks and choosing Part a screen like the one show should appear. From this 3D objects can be created

Example 1 – Hollow half sphere Open a new part, click sketch, then circle on the task bar. Choose the front plane when the planes appear. Draw an arbitrary circle Use Smart Dimensions to show size (either right click on the circle or use the button on the top toolbar Double click on the size and change to 100mm (Left menu bar)

Click Feature on the task bar. Click Extruded Bose/Base Set size (D1) to 50mm Click the green tick (or press enter)

Click Fillet on the task bar Set radius to 50mm Click top face of cylinder Press enter

Go to back of half sphere (click then back) Click Shell on Features toolbar, then click the back face Choose a shelling of 2mm and press enter Now we will make 4 mounting holes in the side of the sphere.

Right click on the top plane on the left-hand panel, select insert sketch. Draw a 5mm diameter circle in the centre of the sphere (a dashed line will appear if you are centred). Make this 5mm from the edge (using smart dimensions).

Now click the features button and choose extruded cut and, on the left panel, through all instead of blind, use the rotation tool to see that it is going through the shape, if not click the arrows beside through all to change the cut direction.

Repeat for the right plane to produce 4 mounting holes Congratulations, you now know Shelling, Extruding, Filleting and Extrusion Cutting. MAKE SURE YOU SAVE YOUR WORK

By yourself create a new object with a 96mm diameter half sphere and some base. SAVE YOUR WORK! (note: duel extrusions will be covered in next lecture but this can be done by filleting the top and edges of some shape).

Assembly In this section of the introduction we are going to assemble the two previous components into one part.

Open a new SolidWorks Assembly Sheet. Click Insert -> Component -> Existing Part On the left, if your part is not there, click Browse and find your part. Open it. (note it will be there if the part is open in SolidWorks).

Adding Parts Now insert your second part the same way Move the second part away from the other (use Move component if necessary)

Joining Parts Rotate your component using rotate component so that they face similar ways – see picture (note that you cannot move the first one you placed).

Click the mate tool (the paper clip) Select the sphere rim, and a parallel surface to align the components Change the join from coincident to parallel click ok (otherwise it might be joint in the wrong place!). Note you might need to rotate your screen to select both, use the rotation next to the magnifying glasses

Now select connection hole inner face of both surfaces to align the holes (see picture, you might have to zoom in to get the face, not the edge – use the mouse scroll). Click OK.

Finally select the inner sphere and outer sphere of the top and bottom pieces respectively to join the parts. Click OK twice to exit mating

Checking design It is good practice to make sure the parts are not overlapping, so click tools – Interference Detection – Calculate. Any overlapping will be shown, this means you have not aligned the parts properly or your measurements are wrong, the parts do not fit together!

Exploding Sometimes it is useful to see how the parts are joining together – this is where the Exploded view comes in. Select Exploded View in the Assemblies Toolbar Click the top of you assembly

Click the Blue arrow and drag up (opposite pointed direction in last slide) Click OK. Now by right clicking on you design name (in left toolbar) you can select Collapse or Explode to change between the two.

Section Cut At the top right of the screen there should be a button like Select this and choose a plane to cut through on the left hand side (note you can do this in the exploded or collapsed views). Select OK to render this setup, to exit this view just click the button again.