- [Instructor] In this video,
I'm gonna be teaching you how to fold, unfold,
and flatten sheet metal parts.
Now in this example,
what I have here is I'd like to take this bend here
and fold it flat, or actually unfold it,
and then make a cut or extruded cut through the part
in its flattened state,
and then fold that part back up.
So to do that, let's go ahead and unfold this bend first.
So go up here to sheet metal.
Come over here to unfold.
So go ahead and choose the fixed face.
That's gonna be this one right here.
And the bend I'd like to unfold
is gonna be this one right here.
Now I can also unbend multiple bends at the same time,
but right now, let's just do that one.
Click on OK,
and that flattens it out.
Now let's go ahead and create a cut feature,
so I'm gonna choose this surface here or this surface here.
Create a sketch.
I'm gonna use the slot command.
And I'm gonna go ahead
and choose the center point of that radius.
Go ahead and create a slot and go ahead
and create a dimension of half of an inch
by inch and a quarter.
There's my slot.
Go over to features, extruded cut,
let's cut that through.
Because we're in a sheet metal part,
we have the option to link to thickness.
Go ahead and check that.
And click on OK.
Now we're ready to fold that part back up.
So go back over here to sheet metal.
Come over here to fold.
Notice this face over here is already selected.
Choose the bend to fold, which is gonna be that same bend.
Click on OK and we're back where we started.
Now if you wanna look at this part in its flattened state,
we have a couple different ways that we can do that.
The first and easiest way to do that
is just come up here to flatten.
Click on flatten, it flattens it out.
It gives you the outside perimeter sketch
showing you how big the flat pattern is
and when you're done with that,
click on flatten again and it folds it back up.
We also have this feature at the very bottom
of our feature manager called flat pattern.
If you click on the roll-down,
you can see here is the flat pattern,
and if you click on unsuppress,
it also flattens it out into that state.
Click on it again, say suppress,
and it folds it back up.
So there are a couple different ways
you can flatten and unfold your parts.
And a lot of times when you're working in sheet metal,
it does save you a lot of time
to unfold some of the bends, add some features,
then fold them back up
so you get exactly what you're looking for.
Otherwise you probably need to do these type of cuts
using multiple features.
So the fold, unfold, and flatten
can really be a great time saver
for working with sheet metal inside of SolidWorks.