In this lesson, we will continue using the same file to

explore the use of flanges and bend overrides.

We already used the flanged tool to create features from sketches,

but the flanged tool can also be used to create features from edges on the model.

With body to active,

start the flange tool from the create pull-down,

then select the lower edge of the top face on both ends of the part,

and drag the arrow down to start creating new flanges.

Before finalizing the new feature,

let's take a look at some of the options.

Looking at the front face on the ViewCube,

you can see that the bend is being added,

and the corners where the new flange meets the existing body are being held back

so that the outside face of the new flange is flush with the end of the existing body.

In the dialog, we can change the bend position,

so that the bend is outside of the original selected edge, a tangent solution.

Or for this design,

we will use the adjacent option,

which will build the new feature without cutting a mieder for relief.

It's important to think about how the rest of the part

needs to be built when selecting options.

These new flanges will eventually fold and

set on top of the previously existing plate so that

fasteners can be inserted into the sheet metal

which will connect to screws passing through the holes in the base plate.

In the previous exercise,

we used radius corners in the sketch to define the bends.

By creating new flanges from the model edge,

we can't simply add new sketches to get the same radius.

We could update the sheet metal rule,

but that's not always the proper approach either.

Instead, we can select bend override in the dialog,

and set the value to be five millimeters to match the previous bends.

As soon as the new value was added,

the part will update, showing the change.

It's also possible to use named parameters to control

the radius of the sketched bend and the bend override.

But for this part, we'll simply enter the values manually.

We also need to establish the correct height for the new flange,

which is the distance the sketch was offset plus the thickness of the material.

So, it needs to be 52 millimeters.

Entering the value, updates the preview,

and we can see that it's perfectly aligned with the top base of the base plate.

Changing our view to see the other selected edge,

all the same rules have been applied to it,

so that now we can say okay to create the new features.

Now, we can begin creating the flanges that will go on top of the baseplate

by selecting the lower inside edges of the flanges we just placed.

As soon as the second edge is selected,

we can begin pulling the new flange in.

And you will see that both are pulling away from the selected edge in the same manner,

even though that means they're developing toward one another.

Looking at the bottom view,

we can make sure that there's enough material

being added to go around the holes in the base plate.

We should also make note that the radius that's being

applied is again the default based on the sheet metal rule.

This smaller radius is just fine,

so we will leave it as is.

If we decide we wanted to make yet another radius five millimeters,

it might be better to just update

the sheet metal rule and all the previous bends to follow it,

to simplify things for manufacturing.

Looking at the part from the right view,

we need to make sure that the new flanges are being developed in

a way that won't require complex cuts in the flat pattern.

So we'll set the bend position to inside to make sure

the edges of the new flange and the last flange remain aligned.

We will leave the value at 40 millimeters and click okay to create the new flanges.

Now that the new flanges are in place and aligned to the base plate,

let's add the holes to the flanges.

To do this, I'll start a new sketch on the bottom of

the baseplate and use the body option for projection,

so I don't have to pick the individual edges.

Under the create menu, along with flange,

you will find extrude,

hole and thread tools.

But since I've projected the edges,

I'll just use extrude.

We'll select the four circles or

the extrusion profiles and pull them up until they go through the sheet metal part.

You can also expand the objects to cut portion of

the dialog to see that we will be cutting body too,

which is the switch plate.

We'll click okay to create the cuts and turn off

the baseplate to be able to clearly see the holes.

The last thing we will do to this overall part is,

round off the exposed sharp corners using

the filter tool which is in the modified

pull-down just like it is in the model workspace.

We'll select the four small edges on the corners,

avoiding the long edges of the part,

and set the radius to two millimeters.

After creating those fielitz,

I use the marking menu to restart the filling tool and

select the sharp corners of the last two flanges that were created,

this time using a radius of five millimeters.

With part largely finished,

it's time to start creating some detail,

which for this part, means creating cut-out for switches.

We'll start by creating a new sketch on the top of the part,

and using the two point rectangle tool from the sketch pull-down to

create a small rectangle near the upper-left corner.

Now, we use parametric dimensions to set the width of

the rectangle to 20 millimeters and the height to 10 millimeters.

Then, we'll add dimensions to set the rectangle 10 millimeters in from the side of

the top base and 10 millimeters in from the edge of the top base.

Next, we'll create a series of the shapes.

I'll select the rectangular pattern tool from the sketch pull-down,

roughly placing a three by three pattern.

Now, let's add a 15 millimeter diameter circle

and use a rectangular tool to create another three by three pattern of it as well.

After creating the pattern,

I'll go ahead and locate that initial circle by placing it 15 millimeters down from

the upper edge and 45 millimeters on the right edge of a rectangle.

Then, we can extrude all the holes through the switch plate.

When extruding these holes,

we need to take care not to use the All option,

so they don't go through the bottom flanges.

We can use the object setting and select the bottom of the face we are going through,

drag a distance or enter the thickness value of the material.

However, a good practice is to use

a named parameter that controls the thickness to set the value.

I'll click okay to create the features for now.

To find the name of the value that establishes the thickness of the part,

go to the modified pull-down and select change parameters.

The value of the thickness was given the name D9.

To have something easier to remember,

I'll create a user parameter named Thickness,

noting the capitalization, and set the expression to two millimeters.

Going back to the part,

I'll edit the extrusion and change the distance value to minus_D9 or to minus thickness,

and say okay to update the feature.

Now, let's save the file,

so we can proceed to the next lesson.

Sheet metal flanges

Autodesk Fusion 360 Integrated CAD/CAM/CAE

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