Fan+How+To+with+pics+edit.pdf

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Computer Fan How To
Modeling a computer fan in SolidWorks
Matt Perez
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In my job there are times when I need a fan to include in an enclosure. Sometimes you can find cad files
of these fans(SW actually has one), but sometimes it’s just easier to model it yourself. This is a simple
representation of a fan. Obviously you can put as much detail into the model as you wish. In most cases
just a block with bolt holes will be adequate but I like to go a little further.
The first step is obtaining a dimensioned drawing of the fan you wish to model. Every manufacturer
offers these drawings. The one I am modeling is an 80x80x24.4mm fan and can be found here.
http://www.delta.com.tw/product/cp/dcfans/download/pdf/FFB/FFB80x80x25mm.pdf
The first step is to start a new sketch on the Top plane. I like to start with a circle centered at the origin.
Immediately give this circle a dimension. In this case it will be 88.6mm as shown on the Mounting Panel
Cutout portion of the pdf.
Next step is to draw a box(use the center point box option this will add some construction lines and
relations that will help you. The first thing I like to do is add an = relation to the top edge and one of the
side edges. This ensure that we have a square(since the fan is square). Then I add a single dimension to
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the box giving it a width of 76.6mm. Because we used a center point rectangle and we used the =
relation everything is nice and centered. Once we start trimming things, these relations will be deleted
but it is a good idea to keep this in mind when modeling.
Next go ahead and trim away the unwanted sections. You will notice your nice fully defined sketch is
now under defined. That’s okay because we know nothing has moved and there is a simple solution.
When a sketch is under defined you have the option to let solidworks fully define the sketch. Since we
know everything is where we want it, we use Fully Define Sketch and modify some of its options. You
can specify to add relations, dimensions or both. You can also get really specific as to what types of
relations and dimensions you wish to be added. In this case make sure Dimensions is not selected and
only allow it to add relations, then Calculate.(note, fully define sketch is located on the drop down with
View relations and Add Relations.) Using only relations, the sketch is now fully defined. I have kept
relations visible so you can understand a little better what is added. Also note that reference lines do
not need to be fully defined for a sketch to be considered fully defined.
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Next step is to add another center point rectangle. This one will define the outside of the fan which in
this case is 80 x 80mm. Again this is centered at the origin and you want to add an = relation between
one side and the top(or bottom) edges.
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