- [[Narrator] Now that we have a hollow box
that completely encloses the PCB part,
we'd like to split this up into two hearts,
so we can actually open it and access the PCB.
And to do this, we're going to use the split feature.
Open your enclosure master part,
just by clicking on it in the assembly
and pressing open parts.
And we're going to draw a sketch along this long face,
and then we're going to split along that sketch.
So firstly we need to start a sketch,
and if you hover over the default plains
in the feature tree, we want to select the one
that's parallel to this long face.
So for me this is the right plane.
For you it might be a different plane,
but just select the one that looks similar
to these videos here.
So left click on the plane
and then press sketch.
So now we're sketching on that plane,
and we want to go to a Normal To view.
So you can just click Normal To on this small menu here,
if you don't have that menu open,
you can always just press space bar to open it.
Then let's go to the sketch tab and select the line tool.
And we want to choose a midpoint line.
So put a check in this box here.
This means that the line will extend equally
into directions.
Let's left click on the origin
to start the line, and then just draw directly upwards.
And you should see that if we go straight up,
we get this small, yellow vertical simple.
So left click somewhere beyond the edge of your enclosure
and then press Escape to close the line tool.
But now we can see down here
that the sketch is still under defined
and that's because we haven't set the length of this line.
So to do this, we're going to use the smart dimension tool.
Select the tool, and then just left click on the line
and just drag outwards and type in 130 millimeters.
So now the line should be fully defined.
You can see down here it says Fully Defined.
So you can press escape to close the smart dimension tool.
If your sketch isn't fully defined, it might just be that
we've missed that automatic vertical relation.
So to fix this, all we need to do is select that line,
hold down Control, and then left click
to select one of these outer lines.
And then down here, just click on parallel.
So when you're happy,
let's exit the sketch by clicking up here in the top right.
Now we're going to use this sketch with a split feature
to split this body.
So to find the split feature,
just go up to the top, click on Insert, Features, Split.
We can also find it using the search box up here.
So to use this, firstly click on the dropdown here
and make sure you're on commands,
and then just start to type in the name
of the tool you want.
Say for example,
start to type Split and we can see their split at the top
and you can just click on it directly up here
to open the tool.
So now we're using the Split tool,
and the good thing about SOLIDWORKS
is it often tells you exactly what to do.
So up here it says we need to select a sketch
and we're going to use that sketch that we just drew.
The first thing we need to do is make sure you're in this
trim tools box.
If it isn't blue, just left, click in there
and then we just need to select our sketch.
So just move over in the graphics area and left click on it.
And now we can see the sketch has appeared here.
So let's press cut part.
Now this body has been split into two separate bodies.
If we put a check in the top box here,
we can see one of these changes color,
and that indicates which one we're working with.
Then if we double click here where it says none,
we get this popup box,
and this allows us to save this body out as a separate part,
which is still linked to this parent part.
To make sure you're in your exercise folder,
you should be in there by default
and then we can just write in a new name.
So let's call this something like Enclosure Top,
and then you can just press Save.
So now you can see the name has changed here on the left
and the label has also changed here in the graphics area.
So now we're going to do the same for the other half.
So firstly put a check in the box,
and then just double click where it says none.
And let's call this one Enclosure Bottom,
and then press Save.
And again, the label changes.
Now all we need to do is click on the green tick up here.
Sometimes you have to click this twice.
Just seems to be a little bug that solid works has.
But when you click it,
SOLIDWORKS will work for a few minutes.
You might get some popups like this.
If you do, just press yes.
And then when you're done we should be back
in the original parts
and you can see we now have the split feature at the bottom
of the feature tree.
But now if we use Control Tab
to go through our open documents,
you can see we've got these two new open documents
and if we go to those we can see
they are the actually the two halves of the enclosure.
And if you were to go to your project folder now,
you shouldn't also see two new files in there.
So let's Control Tab to go back to our enclosure assembly,
and then we can just save everything
by going to File, Save All.