This is a short tutorial on the first part of Lab number 20,
the functionality of Solidworks.
Let's start with a new file, a part file, press ok,
and first thing you want to do is to make sure
that we are in the correct unit.
Right now it's in inches, pounds and seconds, so click on this
and change to millimeters, grams and seconds.
Then we open our sketch toolbar,
click on sketch to start sketching.
It's going to ask us the sketch plan, select the front
and then let's sketch a rectangle,
with lower left corners of the origin,
right here in the upper right hand corner is some arbitrary
point somewhere here.
Don't worry about the dimensions.
The blue lines mean that the edges are not put completely
dimensioned, which is under defined, so use smart dimensions
and change this dimension to 100 and accept that.
Using smart dimensions again, this side here;
we're going to change it to a dimension of 65, accept that
and then accept to close the smart dimension.
Now later on if you want to change dimensions
of something set to 65, just double click the 65
and you can change it this time to 60,
which is really what we want, so from 65 to 60.
A nd then we exit sketch, and we go to features,
extruded boss base as our first base feature here.
I used a current sketch in the extrusion.
We want to use the following conditions - blind,
and a depth of 50 for the depth.
So change it to 50 and then press accept.
And in our feature three manager,
you can see that this created extrude one on this list
over here; extrude one.
Now let's change the display style
to what is called the hidden, with edges shown
so that we can see all the edges because we're going to need
to identify them later.
Then we go to select, the feature select and click
on the four vertical edges, this four that we're going to select
and make sure that the select radius is correct
and it should be 10, and then just accept,
and that simple step is selected so vertical edges.
Next thing we want to do is we are going to create a shell.
But before we do that, let's change back to our view here,
our view style, display style, and then click on shell,
then select the top face as the face were shelling,
and then set the correct width to five for thickness.
And that created the shell from our solid.
So it made it hollow.
The next thing we're going to do is an extruded cut feature,
by starting on sketch again, and we're going
to select this right plane here as our sketch plane,
and we're going to change our view direction to normal too,
so that we're viewing that sketch plane perpendicular
to our line of side, so we can easily create.
Now I'm going to sketch a circle.
I select an arbitrary location of the center and the radius.
And then I'm going to smart dimension the vertical location
of the center of the circle to 40,
and then the horizontal location from the center
to this edge here, going to put that dimension here to 25,
and change that to 25.
So that's the correct location
of the sketch on the right plane.
So I exit sketch and then I go to features, and extruded cut.
It's going to be working on the current sketch, sketch two.
Extruded cut, and I want to make sure that the condition is
through all, it's going to cut through all the entire solid
and accept, and let's change our view to isometric or trimetric
so we can see it in 3d as a solid.
So that really is it for creating our first solid.
Now you're going to repeat the similar steps to do,
to create the switch plate and then the third part
of the lab is, you're going to follow tutor one.
So we're going to open the resources, Solidworks resources,
and we're going to go to tutorials, and then you're going
to go to lesson one, which is on parts.
So click on this and it will give you step-by-step
instruction on how to create this part file called
lesson one.
So let's start the tutorial and if you can see,
it has specific instructions.
It even has icons so if you don't understand or know
where to find this, click on that icon and it will tell you,
point you to the right icon.
So for instance, I don't know where to find the save icon
and I just click on this and then just follow it
and then once you've done this, you just click on next
and complete the drawing.