In this case study, we will be creating this
honeycomb pattern which gradually fades into nothing and flushes with the surrounding
face. Take note that I'm only going to focus on creating the honeycomb pattern and not
the whole cover. To speed up the patterning process and the features associated with it, I
will be demonstrating with a pattern that is less dense than what is shown here. Let's
create the base sketch on the top plane. This will be a rectangle centered on the origin. Begin the extrude command and extrude downwards. With that, this face is in line with the top plane. Hide the base body for the moment. We will start
a sketch on the top plane for the honeycomb. Let's create a hexagon centered on the origin.
Go to create, polygon, circumscribed polygon. Set a vertical constraint on this edge. Draw a line from the center
to the midpoint of this edge. Draw another line from the center
to the midpoint of the adjacent edge. Convert both lines into construction. These will
serve as directions during the patterning process. I personally try to avoid doing patterns within
sketches as I like to keep them simple. My plan is to use this sketch to produce a thin extrude.
After that, I will perform a rectangular pattern of bodies. Start the extrude command and select
the thin extrude option. We want to extrude this slightly below the top plane. To do that, go
to the start option and select offset. Set an offset of -1 millimeter. I will explain
later why we need this offset. Adjust the distance and wall thickness. In this case, I will set the wall location to side
1 so that it thickens inwards from the profile. Go to create, pattern, rectangular pattern. For type, select bodies and select the body. For directions, click on the select
box. Bring back the honeycomb sketch. And select the two construction lines. For distance type, set to spacing. For
both direction type, set to symmetric. Adjust the quantity and distance. I have adjusted the spacing in a way
that causes the bodies to exactly overlap with each other, so that we
can maintain the same wall thickness throughout. Unfortunately, there is no option to
join all these bodies within the pattern command. Let's bring back the base body to take a
look at where the pattern is relative to it. In your own designs, you should adjust the
pattern according to where you need it to be. Hide the base body. Now would be a good time
to save. Box select all the honeycomb bodies. Go to modify, combine. Set the operation to join and
combine all these bodies into one. Let's bring back the base body to take a
look and compare it with the finished model. Looking at the finished model, if you
observe the honeycomb pattern from the side, it sort of rises up and down like a wave. We
shall use a spline to define this profile. Notice also that the pattern is at
a 45 degree angle to the horizontal. Go to construct, plane at angle. Select the y-axis and adjust the angle to -45. Start a sketch on this plane. Draw a horizontal line. Control select the endpoint and the origin
and add a horizontal constraint. Draw a vertical line from the origin and convert it to a center line. Begin the mirror command. The centerline is
automatically highlighted as a mirror line. Select the horizontal line as the object to mirror. These three points will form
the scaffold for the spline. Begin a fit point spline and
snap to these three points. Click on the horizontal/vertical constraint and click on the center spline
handle to make it horizontal. Click on the spline to reveal the two spline
handles at the sides. Adjust each spline handle slightly until they turn blue. In my experience,
I find that this reduces the possibility of the spline warping when you impose a symmetry
constraint. Begin the symmetry constraint and select the end point of this spline handle.
When you hover the cursor over that point, it should turn white. Click on that point.
Do the same for the other spline handle. Lastly, select the centerline. With this, both the angle and length of both spline
handles will be mirrored across the centerline. Add a tangent constraint between
the spline and the straight line on one side. This will be mirrored
also. Dimension the spline handles and dimension the height of the centerline. Confirm the sketch and bring back the honeycomb. When you are doing this sketch, the overall sketch
should exceed the extent of the honeycomb pattern. Activate the surface tab. Go to create,
extrude. Select the sketch as the profile and create a symmetrical extruded surface. Adjust the distance until it covers
the honeycomb pattern completely. Hide the surface body for the
moment. Activate the solid tab. Select the top face of the honeycomb
pattern and begin the extrude command. Let's bring back the surface
body and look normal to the sketch plane on which the spline was created. We want to extrude up to the
surface body. Remember earlier that the honeycomb was extruded
with an offset from the top plane. Without that offset, the extrude to object would fail
as you will be asking the command to extrude a zero thickness solid in the areas on either side
of the spline. So this is why we needed that offset. For extent type, set to to object. From the
bodies folder, select the surface body as the object. This surface body will act as a
limiting surface for the extrude. Let's confirm and hide the surface body. Bring back the base body. Let's use the sidewalls of the
base body to trim off the excess. Go to modify, split body. Select the honeycomb as the body to split. For
splitting tool, click on the select box and select this sidewall. If you hover the cursor
near an edge, you can see the whole body getting highlighted. If you click at this point, you will
be selecting the whole body as the splitting tool, which is not what we want. I would advise you
to zoom in and make sure that you hover the cursor directly over the face. Make sure that
only the face is highlighted before selecting. We can select multiple faces as splitting
tools. To fully cut through the body, we need to extend. Control select the two excess bodies,
right click and remove. You can see that the honeycomb pattern on either side
of the spline flushes with the base body. However, since it is still a separate body, you
can see these edges. We need to combine these two bodies. Go to modify, combine. And combine the
honeycomb and the base body. When the combine is done, the effect does not look that impressive
due to the visibility of the tangent edges. It will look better with the shaded view
turned on. Or you can go into the render workspace. The transition effect should also
look better with a denser honeycomb pattern.
