- [Instructor] We currently have a cavity for the joining
lip in the top half of the enclosure only, and we want
to add a corresponding feature to the bottom half.
Open the bottom half part just by
clicking on it and pressing open part.
And we're going to carry out a similar procedure
to how we cut the lip in the top half.
So start a sketch on this mating face
just by left clicking and pressing sketch.
Then select one of these inner edges
and right click and press select tangency.
So now we have that entire loop selected.
Now we're going to use the convert entities tool,
and this basically converts any selection
into new sketch entities.
So from the sketch tab, just click on convert entities.
And now you can see we have those new lines in the model.
Select all of those by pressing control A
and now we're going to use the offset entities tool.
So from the sketch tab, click on offset entities
and write in 1.25 but don't press okay just yet.
Firstly, just make sure you don't have
any of these construction geometry options selected.
Basically, these options turn either
the off set line or the original line
into construction lines, and we don't want that.
Depending on your version of SolidWorks,
this might be worded slightly differently.
It might say something like make base construction,
just make sure you don't have that selected,
write in 1.25 and then press okay.
We made these lines 1.25 because it's still
a pretty decent wall thickness, but it gives us
half a millimeter of clearance from the lip.
You might remember that was 1.75.
And when you're printing parts like this
that fit together, you should always
leave a small gap between them for the printer tolerance.
Usually about half a millimeter like this is okay,
but it really depends on the parts and the printer.
Now we're going to do an extruded box base.
So from the feature tab, select extruded box base,
and we're just going to extrude 1.5 millimeters upwards.
You might remember that the lip in the other half
is two millimeters deep, so by going 1.5 upwards it gives us
that half millimeter clearance that I just mentioned.
Press okay, and now we've got a lip all the way around
and we can rename that feature just
by doing a slow double click on it and let's call it lip.
Then save your part and we can go back
to the assembly by pressing control and tab.
So if we go to a cross section view,
at first glance this looks pretty good.
We've got a lip here and then we've got the cavity
and we've got that half millimeter clearance between them.
But if I close that view, there's actually a problem.
Spin your model around and see
if you can see what the issue is.
So the problem is that the lip goes
all the way around, so it actually clashes
with these ports like here, here, and here.
So we want to make the lip only where the cutouts aren't.
But we can fix this.
So let's edit the lip feature.
So from the parts tree, make sure you have
the enclosure bottom part expanded.
Then go down to the lip feature,
click on it and press edit sketch.
So now we want to add these lines into the sketch somehow.
So we only cut out where the side port cutouts aren't.
And to do this we can use the convert entities tool again.
Firstly we just need to select these edges
and then we can press convert entities.
Because this top part's semi-transparent,
it can be quite hard to select them
if there's something behind them.
So what you need to do is rotate your model around
so there's nothing behind it, and
let's start with these two on the end.
So just select that upper edge, then hold down
control and select the opposite side.
And then just press convert entities
and you can see that those edges
are projected onto the sketch.
And then we just need to do the same on the other end.
So let's spin it around so there's nothing behind it.
Select that edge, hold down control,
and then select that edge and then press convert entities.
And now those lines are added there.
And then there's just six more on this side,
so there's two for each port.
Just take your time and select all of them.
Now you might have to rotate around to be able to see them.
So there's two more here in the middle.
Make sure you keep control held down
so you can select multiple edges,
and then there's the final one.
So press convert entities and then
those are added to the model.
And if we look from above,
you can see them a bit more clearly.
So now we can exit the sketch by
clicking up here in the top right.
And you'll get an error message like this.
The problem is that we've now got multiple
profiles within the same sketch.
So SolidWorks doesn't know which ones we want to extrude
so it just throws up this error.
But we can fix this pretty easily.
Click on the bottom on exit sketch and rebuild anyway.
And you might have to close these small pop ups at the top.
So now we can see the lip feature has disappeared
and the feature's actually failed.
We've got this warning message on the left.
But we can fix this.
So just click on the lip feature and press edit feature.
And now we're just going to choose
which areas we want to extrude.
Go all the way to the bottom on the left here
and click in the selected contours box.
And then just zoom in on your model,
and we just want to choose which areas we want to extrude.
So the first one is this area in the corner.
So just move your mouse in between the lines
and then left click to select it.
So now we can see on the preview
we are extruding that section.
Then let's do the same on this top corner.
So just zoom in and then click in between the lines.
Then we can do the same on the bottom corner.
And just take your time and select the correct places.
And then finally, there's just
these two small straight sections.
So we've got those selected and then press okay.
So now you can see we've only got
the lip where the cutouts aren't.
Then we can exit editing the part, and if you spin
your model around, you can see the ports are all now clear.
So everything looks good, so we can press
control S to save our assembly.