- [Instructor] The assemble is now almost finished,
but we're just going to add some final finishing touches
and the first of these is going to be some text.
There's many reasons why you might want to add text,
maybe just for your own personal branding,
or you want to label these ports,
or add a warning, or something like that.
Open your top part
and we're going to add text into this open area here.
But you can use these principles
to add it anywhere in your model.
Firstly, start a sketch on this top face
just by clicking on it and pressing Sketch,
and then choose the Text tool from the Sketch tab.
It's this one that looks like an A.
Then just type the text you want
in this text box on the left.
So I'm going to write something like Enclosure 1.
You can write anything you want,
maybe a name or something like that.
You can see the text appears here in the graphics area.
And anywhere that we left-click
the text will move to that position.
But this isn't a very accurate way of placing the text
and it's not easy to change the angle.
So if we use a construction line or a centerline
then we can specify exactly where we want the text.
To do this close the Sketch Text tool
by click on the green tick
and then choose a centerline.
So click the drop-down next to the Line tool
and choose Centerline.
Now just draw a line wherever you want the text.
So I'm going to draw something like this,
and then you can use Smart Dimension
to specify the exact position of that line.
So let's go 15 millimeters in this direction
and 20 in this one.
So now we need to find a way to anchor this text
onto that centerline.
And to do this you need to open the Text tool again.
So hover your mouse over the text
and you should see that it changes to an A symbol.
This can be a bit fiddly,
so you might need to zoom in a little bit.
So move your mouse over the text,
when you get that A symbol just double-click,
and now the Text tool is open again.
Then click in this Curves box at the top,
make sure it's blue,
and then just choose your centerline.
And now you can see the text goes along that line.
We can change the direction of the text using these buttons,
and we can change the side of the line using these ones,
and we can change the alignment using these ones.
So this looks pretty good in terms of position,
but it's probably a bit too small.
If we're going to 3D print this
then we don't want to make the details too fine.
So to adjust the font and the size
all we need to do is uncheck
this Use document font box down here
and then click on Font.
Now you can use any font that you have on your computer.
So I'm going to try something like Ariel,
I'm going to make it Bold, so it prints nice and clearly.
You can adjust the size here.
So let's try something like 16.
And you can see the text doesn't update
until we press OK.
So that looks a bit better,
it's probably a little bit too small still,
so I'm going to click Font again
and then change it to 24.
When you're 3D printing text like this
ideally the smallest part of the letters
should be about one millimeter across or larger.
So when you're happy let's press OK,
close the Text tool, and then exit the sketch
by clicking up here in the top right.
Now we can use this sketch just like any other sketch.
So we could create an extruded boss
to raise the letters up
or an extruded cut to cut them down into the top face.
It's really up to you.
I'd probably recommend cutting them,
just 'cause it gives them a bit more protection,
stops them getting broken off or worn down.
So to do this let's select the sketch
in the feature tree by left-clicking,
go to the Features tab, and just press Extruded Cut.
And let's do a Blind cut, 1.5 millimeters down.
Press OK and now we can see the text
is cut into that top face.
And this was another reason
why we made the walls three millimeters thick,
just gives us plenty of space
to cut any details like this down into it.
Then if I go to the Evaluate tab
and choose the Measure tool and I zoom in
we can see the letters there are about one millimeter thick,
so they should print fine.
So if your text looks good here
you can just rename the feature in the feature tree
by doing a slow double-click
and let's call it something like Text Cut.
If you need to adjust it
you can just click on the feature and press Edit Sketch,
then press Control + S to save your part.
And if we use Control and Tab to go back to the assembly
now we can see the text there.
So you can press Control + S to save your assembly too.