>> This lecture is on three construction techniques
on SolidWorks.
They are the loft, the revolve, and sweep.
And there are techniques similar to this in AutoCAD as well.
So, let's start with the loft.
Loft blends multiple profiles together.
A loft feature can be a base, boss, or a cut.
And to create a simple loft feature,
what you do is you create the planes.
It's required for the profile sketches.
So, you create the series of sketches on different planes.
And then a sketch profile on the first plane.
Sketch a profile on the other remaining planes like this.
So, here is the first sketch plane is the front and parallel
to that is plane one, plane two, and plane three.
And you have different profiles on it.
And then you loft it.
Selecting each profile in order
and examine the preview curve and the connectors.
The dots here.
And click OK.
And it will create for your lab, the handle of the chisel.
More information about loft.
It's very important to be neat
so that the program doesn't get confused
on how you want to create a loft.
You need to select the profiles in order.
That they are connected.
Click corresponding points on each profile.
The vertex closest to the selection point is used.
And you can drag the connectors
to improve the connection if you want.
A preview curve connection the profile is displayed right here.
And you can drag the connectors.
Review the curve in order to address adjustments
if needed before clicking OK.
Neatness counts.
You may have unexpected results if you have some errors
like this for instance.
It's twisted.
And that happens when your,
the points on your profiles are not the corresponding points
that they should be.
Neatness counts.
You can have, rebuild errors, for instance,
if your profiles are in the wrong order.
So, here's one, two, three, four rather than going this way.
So, to create, so let's go through the steps.
To create an offset plane, hold down control.
And then drag the front plane
in the direction you want to offset it.
This is a common technique in Windows.
The property manager appears.
And then you select this offset distance.
Change it to 25 millimeters.
And click OK.
And what happens is here is the original front
that you're trying to offset.
It creates this new plane called plane one that's
at the distance of 25.
You can do a similar technique
to create the other two profile planes.
Plane two at a distance of 25 from plane one and plane three
with a distance of 40 from plane two.
Verify the positions of the planes by clicking
on the view, on view planes.
Double click on the planes to see their offset dimensions.
After you create the planes, you create, you sketch the profiles.
So, the loft that we're going
to create is based on four profiles.
Each profile is on a separate plane.
To create the first profile, this is on the front view
and we sketch a square.
It might be better to make your square right in the center.
The center of the square is right in the origin rather
than the origin being on one of the vertices.
By selection sketch center rectangle at an equal relation
to the horizontal and vertical lines.
It becomes a square.
And then add the dimension on one of the sides automatically.
The other sides would also be the same dimension.
And then sketch the remaining profiles.
Opening a sketch on plane one.
Sketch a circle and dimensions shown here.
The center is at the origin,
which is at the center of the first profile square.
Exit sketch.
Open sketch on plane two, and you're going to create a circle
that is circumscribing the original square as shown.
So, the corners of the square should be touching the circle.
And then exit sketch.
And then the last profile is simply copying the circle
from plane two to plane three.
So, you click edit copy or click copy on the standard toolbar.
Select plane three
in the Feature Manager design tree area.
Click edit, past.
And then a new sketch four is created on plane three.
By the way, when you're copying sketches,
external relations are deleted.
For example, when we copied sketch three,
the geometric relations containing,
or locating the center of that circle
and defining the circumference were deleted.
So, sketch four is actually under defined.
So, we need to define it, fully define it
by making it co-radial, adding the co-radial relation
between the copied circle and the original circle.
If you sketch a profile on the wrong plane,
move it to the correct plane using edit sketch plane.
Do not copy it.
To move a sketch to a different plan, right click the sketch
in the Feature Manager design tree and edit sketch plane
from the shortcut menu.
Select a different plane.
And click OK.
It moves it to the correct plane.
Now, what the loft feature does, it blends together the profiles
that were created in order to create the handle of the chisel
that we're making in our model.
So, you click on the lofted boss/base
on the feature toolbar.
And here's an illustration of how you create the loft.
Select each of the profiles on plane, on the front plane,
plane one, plane two, plane three.
Examine the preview curve right here.
Make sure that it makes sense and they're correct.
The sketch, and make sure
that the sketches are listed in the correct order.
Sketch one, sketch two, sketch three, and sketch four.
You can move specific sketches by doing the up
and down arrows here in order to arrange them correctly.
And then you click OK.
And what happens is you created a loft
by connecting the four profiles that we made.
We're going to create another loft feature
for the bit of the chisel itself.
So, the second loft feature is composed of two profiles.
One sketch five and one on sketch six.
To create sketch five, we're going to create,
we're going to select the square face of our sketch plane.
Then we open a sketch and click convert entities.
So, what it does is the boundaries
of this face becomes our sketch plane,
our sketch, which is a square.
Then I just sketch.
For sketch six, we offset plane four behind the front plane.
So, it's at the distance of 200.
You can create it the same way that you created planes one,
two, three by holding down control and dragging front plane
in the direction you want it to go.
And then you can adjust the distance to 200.
Now, open a sketch on plane four.
And on this sketch plane, you create this narrow rectangle
with these dimensions.
Also center rectangle and exit the sketch.
Then you create the second loft feature by clicking
on the lofted boss/base on the features manager.
This icon here.
Select the two sketches.
Sketch five and sketch six down here.
And example the preview.
In this case to be the, they're being connected
by straight lines because there's only two profiles.
And click OK.
And lofted chisel looks like this now.
Now, revolve feature.
A revolve feature is created by rotating a 2D profile
around an axis of revolution.
You did a similar thing in one of our labs in AutoCAD.
You created a 2D profile.
And then you selected an axis of revolution and revolve it
in order to create a solid of revolution.
It works exactly the same way.
The profile sketch can use a sketch line or center line
as the axis of revolution.
So, here's the center line.
Or it can be one of the edges of the sketch.
The profile sketch cannot cross the axis
of revolution like this right here.
So, it could be right on an edge or outside.
This will create a hole in the middle when you revolve it.
This one will make it completely solid.
This one is not allowed.
You select the sketch plane.
And then you sketch the 2D profile here using these
dimensions given.
Then you can also sketch a center line, which is optional
because I said you can use this line itself
as your axis of revolution.
The axis of revolution must be in the sketch with the profile.
It cannot be in a separate sketch.
It should be part of the sketch that you made.
The profile must but cross the center line.
We already talked about that.
Then you click revolved boss/base.
This icon here.
Specify the angle of rotation.
We want it to go around completely, 360 degrees.
And it creates this solid of revolution
as our starting feature, base feature
for the lab that we're making.
Now, finally, the overview, the sweep feature.
It is created by moving a 2D profile along a path.
So, it's like an intelligent extrude,
this extrudes usually along a straight line perpendicular
to the profile itself.
Here it is sweeping it along a specified path.
A sweep feature is used to create
in our lab the handle of a candlestick.
Oh, it's not a lab.
It's a candle stick.
The sweep feature requires two sketches, the sweep path,
here's the path here along which you sweep the section.
The sweep path is a set
of sketched curves containing the sketch, a curve,
or a set of model edges.
The sweep section must be a closed contour.
And our example would be an ellipse.
The start point of the path must lie
on the plane of the sweep section.
And the second, path,
or resulting solid cannot be self-intersecting.
Again, it will get confused.
Now you want to create your solid as you sweep it.
You can first create the path.
And then you make the section.
Create small cross sections away from the other part
of the geometry because you can simply move it later
by using coincident or pierce relation
to the end of the sweep path.
That will actually guarantee that the beginning
of the sweep path is in the same plane as the sweep section.
So, let's create the sweep path.
Open a sketch on the front plane.
Sketch the sweep path using the line
and tangent arc sketch tools as shown here.
So, I see some lines and tangent arcs
to create this using the dimensions shown.
And then close the sketch.
Then create the sweep section.
Open the sketch on the right plane, for instance.
Sketch the sweep section as an ellipse with these dimension.
Major axis 35.
Minor axis 10.
And made the major axis horizontal
by adding the horizontal relation.
Dimension, smart dimension to the correct dimension.
And then you move this sweep section
by adding a coincident relation between the center
of the ellipse and the endpoint
or the beginning point of the path.
So, it makes coincident.
So, the starting point here is
in the same plane as the ellipse.
And you close the sketch and select swept boss/base
on the feature toolbar.
There's the symbol.
Select the sweep path.
Sketch three.
And select the sweep section sketch too.
And then click OK.
And then the result is this swept feature that serves
as the handle of our candlestick.