- [Narrator] The lofted bed command allows us
to create complex geometry inside
a Solidworks sheet metal.
To get started, all we need is a couple different sketches
on some planes, and we have to have an open contour.
So here's a part that we're going to be creating.
And I'm going to be starting this part from something
that looks like this.
So I've got a sketch on the top
and I got a sketch on the bottom.
And we're going to loft between these two sketches.
My second example is going to be something
that looks a lot like this.
It's going to open contour and again,
that's going to be starting from
a file that looks like this.
So let's go ahead and jump right in.
So first things first, let's go ahead
and close this file here,
and close this one right down here.
And then let's start from my first example here.
Alright, now before we jump into the loft bend command,
I want to show you what I have on these sketches.
So I'm starting off with sketch number one,
and it has to be an open profile.
It can't be a full closed circle,
so what I did is I added a half of a degree of a gap,
right over here.
So you can see it's not actually closed,
it's one circle that's going around here
with a little gap in it so it makes it an open profile.
And then exit out of that, and let's take a look at
the plane number two, which I just pushed up above
the original plane.
And then I sort of sketch on there.
And heres my sketch.
And again, I've got a very, very small gap right here.
And you can see I've also radiused the corners,
so you have a nice smooth part.
Sometimes sharp corners will cause issues,
so in this case here, everything's rounded,
and we have a small gap.
Click on okay, and there are the requirements
for starting a lofted bend.
Alright now, jump over to the lofted bend command.
Now we have two options.
We have a bent part or a formed part.
Now something like this has to be a formed part.
So make sure that you do choose the formed part.
Otherwise it probably will fail.
Grab our profiles, let's choose this one down here,
going up to this one right here.
And I can see a nice preview of exactly
what's going to be happening here.
Alright we can choose the thickness of the material.
So right now it has quarter inch thick materials.
Doesn't really matter as long as you're not making
a thickness that's too large
for the bend radiuses that you're using.
I'm going to go ahead and use the defaults here.
Click on okay, and there's our new part.
So pretty handy and pretty cool looking part.
It happens to be very easy to create using that
lofted bend command.
The main requirement is though that we have
at least two contours to create the shape from
and they have to be open contours.
And ideally you have that line of where they're
going to be connecting that sheet metal together
in pretty much a straight line.
Alright, let's jump over to my secondary example.
Which is this one here.
Pretty much the same thing,
I've got a couple different open sketches.
And notice they have the same amount of points.
And that generally is a good idea because
you're going to have these individual bends
and you want to make sure they stay
kind of in a straight line.
So when you form that part, everything makes sense.
It would be really hard to make a part
that went from four bends, to three bends for instance,
unless you're just making a completely thermal form part
or something like that.
But in this case here, let's see what happens.
So we've got sketch number one, here it is.
And let's take a look at it.
I've just added some nice radiuses down here.
And we're using a mirror command so the right hand side
looks like the left hand side.
And pretty much exactly the same thing
on the secondary plane here, I created sketch number two.
And it looks very similar.
Alright, now we're ready.
Alright, so let's jump in here and create a lofted bend.
And that's going to be going from this one here
up to this guy over here.
And you can also try switching over to the bent option.
But normally, if you do bend options
you're going to have a few more options here
and it's not as likely to work.
So generally I stick with the formed part here,
and we're going to define the thickness,
and click on okay, and just that easily,
we're able to create a nice part.
In this case here actually looks a little bit thick
because the bend radius
is causing an issue, because our bend radius is too small
in this piece here.
So if we change that,
maybe .125,
you get a preview, because it's not blowing out that radius.
Now we should be able to click on okay,
and there's our part.
So definitely make sure you're putting
the correct bend radiuses in,
and make sure the thickness corresponds
to that bend radius so that you don't pinch those corners.
That's pretty much how to use the lofted bend
in Solidworks sheet metal.