>> This is a short lecture
on creating assemblies in SolidWorks.
We're going to illustrate this by first creating Tutor 2,
as instructed in the lab.
And in creating Tutor 2, you're going to start
with this base extrude rectangular feature.
And then we're going to fillet these four edges as shown.
And then we're going to shell.
Specific instructions are given
in the tutorial on SolidWorks itself.
And then we're going to do a cut extrude to create this lip.
And, in creating the cut feature for the lip,
we're going to create this sketch that's composed
of two curves by converting entities
that are already existing.
The outside of the curve.
And then offset it to create the inside curve.
Rather than drawing outlines by hand for these curves, we use,
we copy existing geometry from the shell feature.
This technique is fast and easy
because you already have your entities.
You're just offsetting them and copying them.
It's more accurate because the sketch entities are copied
directly from existing geometry.
And it's also intelligent.
It is very important for, a very important feature of SolidWorks,
that if we change the, make some changes in the body itself,
the sketch gets updated automatically.
So just to illustrate the conversion
of existing entities into sketch features.
It copies one or more curves into the active sketch,
but projecting them onto the sketch plane.
The curves can be any edges of any existing face.
Entities and other sketches can also be for copying.
It's fast and easy.
All you have to do is click on this tool.
Select the face for the curve that you're trying to copy.
So in this case select the sketch plane.
It's right here, this face.
And we open a new sketch.
And we select the face or curves that's we want to convert.
In this case the selected face.
And then we click on this toolbar, convert entities
on the sketch toolbar.
So this converts existing geometry
into sketches in the sketch plane.
The outside edges of the face are copied
into the active sketch.
And then the sketch is already fully defined.
No dimensions are needed.
It's just simply copying something that's
already existing.
And then we're going to create the inside curve
by offsetting the outside curve.
Clicking on this offset entities on the sketch toolbar.
Enter the distance value for the offset, 2 millimeters.
Select one of the converted entities.
And then select "chain" so that the offset goes all the way
around the contour.
So the system generates a preview, the green image here
of the resulting offset.
And you can change the direction of offset
by simply positioning your cursor on the right side
of the entity here, offsetting.
So we need to move the cursor inside a contour
because we're going to, the offset is going
to be a smaller copy of the original.
The resulting sketch is already fully defined.
And there's only one dimension that controls the copy.
That is this 2 millimeter offset
that is offsetted inside the contour.
And that will complete this lip here for Tutor 2.
So the Tutor 1 part file is something
that you created in the previous lab.
And this Tutor 2 is sort of, we just went over the steps.
You just follow the specific steps given in the tutorial,
in tutorial resources of SolidWorks.
And then from these two parts we're going
to create... this lab is about creating assemblies.
So we're going to put these two parts together
into this assembly, which we're going
to call the tutor assembly.
An assembly contains two or more parts.
In an assembly, parts are referred to as components,
components of the assembly.
And mates are relationships that are define the relative position
of the different components.
They indicate how the parts align
and fit together in the assembly.
Components and their assembly are directly related
to file linking.
What that means is any changes you make in the components
or the parts will actually automatically update those
changes in the assembly and vice versa.
If you change anything in the assembly,
that actually affects the original components as well.
This is one good feature of SolidWorks as well,
the linking of the files.
Changes in the original part files will automatically
update assembly.
And changes made in assembly will also automatically update.
So here are the steps in creating the tutor assembly.
You open a new file.
But it's going to be an assembly document rather
than a part file.
And then you open the two-part file that you're going
to make an assembly out of.
Open Tutor 1, that drawing that you made from the previous lab.
And Tutor 2, the parts file that we just create,
that you just created to the first part of the lab.
And then arrange these windows.
So this would be where the assembly's going to go.
This is where Tutor 1 is.
And this is Tutor 2.
And to create the tutor assembly, all you have to do is
to drag the part icons into the assembly.
So we just drag them into the assembly document.
And then you can save the assembly as Tutor.
So, for instance, here,
depending on which component you first place
into your assembly file, that first component is placed
into the assembly in a fixed position.
So, if you drag Tutor 1 first, you will notice that this,
there's a letter F in front of tutor.
That means it's a fixed component that cannot move.
If you want to move this fixed component,
you have to first float or unfix it.
After do you that, drag Tutor 1 into the assembly area,
you see the design, the feature manager design tree.
You see Tutor 1 with the letter F, indicating that it's fixed.
And then you drag Tutor 2.
And, if do you that, the feature manager design tree will show
Tutor 2, your assembly, with a minus sign in front.
Indicating that it's underdefined.
That means its position is not, it's still floating.
It's not fixed yet.
And your next task is to find the position
and relative orientation of Tutor 2 with respect to Tutor 1.
Because currently Tutor 2 can move in translation
in two directions as well as rotate about three axes.
So you can move the components by dragging.
The selected component according to its available degrees
of freedom, you can move it.
So, initially, Tutor 2 can move in six degrees of freedom.
Three translations and three rotations.
You can manipulate the position of this unfixed
or floating component.
Rotate and dragging it.
So here's an illustration of the six degrees of freedom of motion
of the floating component.
Translation along X. Translation along Y. Translation along Z.
And then three rotations about each of those three axes.
The way we fix the relative position and orientation
of Tutor 2 with respect to Tutor 1 is
by creating what's called mate relationships.
These mate relationships align
and fit together different components in an assembly.
For the tutor assembly, in order to fix the location
and orientation of Tutor 2 with respect to Tutor 1,
we need to make three mates to be defined.
The first mate is coincident
between this back edge here of Tutor 1.
And the edge of the lip on Tutor 2.
So you want this line here, this edge here
and this edge here to be coincident.
So the name of this mate relationship is coincident.
Meaning they are the same position.
The second mate is coincident again between the right face
of Tutor 1 here, the green face here,
and the right face of Tutor 2.
We want those two to be coincident.
Meaning these two faces are in the same plane.
And the third mate is, so even if these two right planes are
in the same plane or coincident,
you can still rotate Tutor 2 relative to Tutor 1.
So defining the six-step position of Tutor 2,
we create the third mate by using the coincident mate again
between the top face of Tutor 1 and the top face of Tutor 2.
Just to understand how creating these mates fixes the position
and relative orientation of Tutor 2 with respect to Tutor 1.
The first mate removes all degrees
of freedom except for two.
So, when we made this edge here and this edge here coincident,
what that means is Tutor 2 can no longer move up or down
or in the Z direction.
The only translation of motion is along this axis X. And also,
if this edge is coincident with this edge,
obviously Tutor 2 can no longer rotate about the Y,
the vertical, or the Z axis.
It can only rotate along the X axis.
So we have removed all but two degrees of freedom.
And the remaining degrees of freedom,
as a result of making these two edges coincident, are moving,
movement or translation along the X axis, along the edge.
And then rotation around the edge.
The other four degrees of freedom have been removed.
Now, in creating the second mate,
we removed one more degree of freedom.
So, when the second mate was making this right face
coincident with this right face,
so these two faces should be in the same plane.
That means you no longer can move Tutor 2 in the X direction.
The only remaining degree
of freedom is rotating about the X axis.
And, finally, the third mate making the top face
of Tutor 1 coincident with top face
of Tutor 2 removes the remaining degree of freedom.
We can no longer rotate.
Because otherwise those two planes will not be
in the same plane, which is the horizontal plane.
So part of your lab in creating,
second part of your lab creating assemblies,
you will apply mate relationships
for the switchplate part and two fasteners.
You have created the switchplate
and hopefully also the fastener, the screws here.
And we're going to create a switchplate-fastener assembly,
as shown here.
So we will, to fix the position of the fastener relative
to the switchplate, we're going, again, need three mates.
The first mate is concentric.
We're going to make a concentric mate
so that this cylindrical face of the fastener is concentric
with the cylindrical face of the hole of the switchplate.
Concentric means that the center
of this cylindrical hole is the same as the center
of this circular part of the fastener.
The second mate is coincident between the flat back face
of the fastener right here
and the front face of the switchplate.
So we want this to be flush
to the front face of the switchplate.
And, finally, the third mate will be,
we're going to make this flat top
of the fastener right there parallel to the face here.
So that this edge is here,
these two horizontal lines are parallel to the top plane.
And that fully defines the position
of the fastener relative to the switchplate.
Obviously, when creating your assemblies for this,
the first object that you need, the first part you need to drag
into your assembly area will be the switchplate.
That's the fixed part.
Now, for the lab itself,
in addition to those tow assemblies,
let's look at the lab.
So, in addition to Tutor 1 and Tutor 2, the first one
that you create for your assembly.
And the switchplate.
Here is the step-by-step instructions on the switchplate.
Including the creation of the fastener.
And the creation of the mates, concentric,
coincident and parallel.
So, in addition to those two, you're also going
to do another exercise on assemblies
by assembling the mechanical claw.
The files for this are on web access, the part files.
And you're just going to follow the steps here in order
to create a mechanical claw.