In the series of visualisation videos so far,
we have covered the ideas of big picturing and the surface patchwork approach. Today, we
will take a look at the multi-body approach. Here we have quite an interesting design for a
tank or a vessel. Thank you to Josh for sending this design to me. When trying to reverse engineer a model, the
first step is always to pose the question: Can we start with a basic overall shape and
cut it down to this final shape? In this case, the answer is quite clearly no.
Next, let's consider the surface patchwork approach. Can we build this by
building a patchwork of surfaces? Let's try to identify the main faces. There are 3 types
of faces here. We have a cylindrical face here. Straddling across the cylindrical
face are 3 conical faces. And lastly, we have lofted faces capping both
ends. We can definitely build surfaces and trim the excess. But in this case, the
trimming can be quite complicated. It would actually be easier to apply a multi-body
approach. Basically, we will be creating separate solid bodies in the form of a cylinder and a
cone and applying Boolean operations between them. Lastly, we will cap both
ends with solid lofts. Before we start, let's identify planes of
symmetry. There is a plane of symmetry along the right plane. At the same time, recognize
also that there are 3 identical segments. We shall build the center segment,
create a copy on one side, make the loft and finally mirror everything
across the right plane. There is also a plane of symmetry along the front plane. However, making
use of that would actually complicate the workflow as that would require us to build half a cylinder
and half a cone. So we would not be using that. Start with a sketch on the
right plane. Create a circle and extrude into a cylinder symmetrically. Next, we are going to create a profile for
revolving the cone. Start a sketch on the front plane. This will be a right angle
triangle with its corner at the origin. Go to create, revolve. Select
the profile and the axis. For operation, set to new body. We have 2 separate bodies overlapping
each other. Comparing to the final model, we can see a hint of how the cylindrical
face can join to the conical face. From here, we need to make use of boolean operations to allow
these 2 bodies to interact with each other.
By far the most powerful Boolean command we have
is the boundary fill command. However, this can be tricky to use as cell selection is not exactly
user friendly. Go to create, boundary fill. Select the cylinder and the cone as tools. The
boundary fill command computes the interacting volumes between the 2 bodies and offers up
cells for selection. To help in our selection, let's change the environment to dark sky.
This will allow us to more easily see the cells being highlighted. Click on the select
box and start selecting the required cells. For operation, set to new body. We
shall check the remove tools option. This will remove all the remaining
unused volumes from this interaction. Let's check the browser. In one fell swoop, the command has joined the required
volumes and removed the excess. An alternative to the boundary fill command is the split body
command, which I will be explaining here. It is more tedious and requires a good understanding
of how the command works. The geometry involved can be quite tricky to visualise. If you are not
interested in this method, feel free to use the timestamps to skip to the next chapter.
Let's roll back to the point where we had the cylinder and the cone as separate bodies. First,
let's try to remove the excess cylindrical volume that is on top of the cone. We can use
the cone as a cutting tool in this case. Go to modify, split body. Select the cylinder
as the body to split. For splitting tool, click on the select box. When it comes to tool
selection, we can select either a face or the whole body. In this case, we need to select
the conical face. If we select the whole body, the flat base of the cone would also be employed
as a cutting tool, which we do not want. If we hover over the conical face, notice
that it turns a slightly paler shade. If we hover over an edge, the
whole body gets highlighted. So make sure you hover over the
surface before you click. Be sure to uncheck the extend splitting
tool option to prevent this error. Once you confirm, you can see
that a new body has been formed. This is the portion of the body that
has been split out from the cylinder. Let's right click and remove this body.
Let's compare this to the final model. We need to remove this portion of the cone that
is outside the boundaries of the cylinder. This time, we are going to flip the roles around.
The cylinder will serve as the cutting tool. Start the split body command again. Select the
cone as the body to split. For splitting tool, click on the select box. Selecting this face will
not be sufficient in cutting out the required portion. We need to select the whole body. Hover
the cursor over an edge of the cylinder and notice how the whole body gets highlighted. Click at this
point to select the body. Looking at the browser, you can see that 2 new bodies have been
created from the splitting of the cone. We shall remove the unwanted body. Go to modify, combine and combine all
the bodies into 1 single solid. Create a sketch on the front plane. Use this sketch line to split
out the tip of the cone. We shall create a copy of the body on the left
side. This can be done with the pattern command or the move/copy command. Let's use the pattern command.
Go to create, pattern, rectangular pattern. For type, select bodies and select the existing
body. For direction, select the x-axis. Adjust the quantity and spacing. For the lofted end, we shall use
this face as the starting profile. For the ending profile, let's create an
offset plane. Start a sketch on this plane and draw a circle tangent
to the existing cylinder. Go to create, loft. Select the
starting and end profiles. For the tangency options, set both as connected. Combine both these bodies.
And mirror the body across the right plane. As long as you set the operation
to join, any overlapping region would be merged into the final body.
