- [Narrator] The base flange tab feature
is the primary sheet metal creation tool.
This same tool can create three types of flanges,
based upon the input geometry provided.
The most basic is an enclosed boundary,
so let's go ahead and create one of those.
So to get started I need to create
a sketch on a face or a plane.
Now to do that, let's go over here to the sketch toolbar.
Alright, we start with choosing sketch right up here,
and it'll automatically present the
three different planes I can start from.
So let's go ahead and just choose any one of those.
Click on this one here!
And let's go ahead and start creating an enclosed boundary.
So the most basic enclosed boundary is just a rectangle.
So let's go to the sketch toolbar,
grab the corner rectangle tool.
Let's go ahead and start right at the origin,
and then drag out our shape.
Now, it's always best to define the size of your shape,
so notice we've got a couple different blue lines over here,
and a couple different black lines.
The black lines means they're fully defined
and the blue lines means they're undefined.
So notice I can drag this one right to left,
this one up and down, or I can grab that corner.
I can move it around, but I can't move these lines here.
I can try to drag it, but it won't go anywhere,
because it's fully defined, and it's black.
Now if you get a red line or a yellow line that means
it's over-defined, and that can cause
a lot of issues for you, so you either wanna
delete the sketch itself, or delete
the relationship that's been added.
So in this case everything's happy,
so let's go ahead and add a couple dimensions.
So I'm gonna dimension this bottom line here,
type in four inches, and dimension
this line over here, at three inches.
Now for instance if you go over here, and you say,
"Hey, I'd like to add one more dimension here."
And notice it makes everything yellow because it's saying,
"Hey, you've already added a dimension
on the left hand side, and if you're tying to add
another dimension on the right hand side,
that's gonna cause an issue."
So you can either make a driven dimension,
or you can leave this dimension driving.
If you do that, notice it shows up as yellow,
and this dimension over here is highlighted
in yellow as well, showing this is an issue.
So, you're defining this two different ways,
so there's a conflict, and it's unsolvable.
So go ahead, delete either one of these dimensions,
Let's go ahead and delete this one over here,
hit delete on your keyboard, and now it's happy again.
So notice everything is fully defined,
all the lines are black, all the dimensions are black,
and now we're ready to create that base flange tab feature.
But because it's an enclosed boundary,
it's gonna be creating just the base.
So click on sheet metal, click on base flange tab,
and notice we can just define the thickness right over here.
I'm gonna type in something like court range,
so point two five, and then define how you wanna use the
bend allowance, or the K-factor.
So, depending on the system you're using,
you can use either K-factor, a bend table,
bend allowance, bend deduction, or bend calculation.
So a whole bunch of different ways we can do this.
Generally, I like to leave this as K-factor
if I don't know the exact values,
because it's always gonna work if you use it point five,
or if you do know the exact values
for the bends you're gonna be making, go ahead and
use the bend deduction, and then type in that value.
But if you use bend deduction and you put in the wrong value
your features will fail, so don't use this if you
don't know what you're doing.
But again, if you're trying to make it
very accurate flat patterns, make sure you do
use the bend deduction or bend allowance.
Put the exact values in for the exact angles and thickness
of the material you're using, and then you're gonna get
very, very accurate flat patterns that you can
send directly to a laser cutter,
or into the sheet metal shop.
But for right now, let's go ahead
switch that right back to K-factor because we
don't really know those values off the top of our heads,
and we don't really have time to look them up.
The also, the option here to change the auto relief type
from rectangular to tear or obround.
I like the obround one.
And once you have that, go ahead click on okay.
And now we have our very first sheet metal base.