This is my entry for the speaker cover design
contest recently put up by the 3D Printing Nerd. Just a quick overview before we begin. The overall shape was created by revolving
an arc and shelling. There are 3 types of panels here. A honeycomb panel. A 3-tiered triangular panel. And a third panel that consists of 3 concentric
rings. Each of these panels were derived from the
original revolved body. Let's start with the main revolve. Begin a sketch on the front plane. Sketch a vertical line and a horizontal line, with both meeting at the origin. Join these 2 lines with a 3-point arc. Draw a horizontal construction line that meets
the arc at this point. Make the arc tangent to this line. Select the vertical line. We shall turn this into a centerline for the
revolve by going to the sketch palette and selecting the centerline option. Confirm the sketch. Go to create, revolve. Because of the existence of the centerline,
both the profile and the axis get automatically selected. Go to modify, shell. Select the bottom face and adjust the thickness. Start a sketch on the top plane. Go to create, polygon, circumscribed polygon. Center this on the origin. Press tab to activate the field for entering
the number of sides and enter 6 to get a hexagon. Press tab again to switch to the dimension
field. Add a vertical constraint to this edge. Confirm the sketch. Go to modify, split body. Select the main body as the body to split. For splitting tool, click on the select box
and select the sketch. We are now going to split out the triangular
and the ring panel. We can certainly do this with 3 sketch lines
and then use the split body command. I am actually going to try something new here. Let's name the hexagonal panel body and hide
it. I am going to use this body to split itself. Go to modify, split body. Select the main body to split. For splitting tool, click on the select box
and select this face. This face is a result of the split body done
using the hexagonal sketch. If we extend the splitting tool, the resultant
cutting line would automatically be collinear with the edge of the hexagon. Typically, we would use a separate entity
to split a body. In this case, we are leveraging on the body's
own face to cut itself. Repeat this process another 2 times using
these 2 faces as cutting tools. Let's name the 2 panels. We do not have any use for the other 2 bodies. Control select them and right click. Instead of deleting them, we want to remove
them. This removes the bodies and creates steps in the timeline. Take note that deleting bodies would actually
delete any referenced features in the timeline so do not use that. Let's hide the triangular panel for the moment
and focus on detailing the ring panel. We are going to use the new thin extrude feature
with open profiles to make the cut. Begin a sketch on the front plane. Draw a horizontal line. Dimension it to 7 mm from the origin. Make this end point in line with the origin
by imposing a vertical constraint on the 2 points. Dimension the length to exceed the body. Begin the extrude command. Select the thin extrude option and select
the line as the profile. Let's make the direction symmetric and control
the distance such that it completely cuts through the body. Adjust the wall thickness. In this case, we are adjusting the thickness
of the cut. Make the cut symmetrical about the sketch
line by setting the wall location to center. To create the effect of concentric rings,
we are going to pattern the cut. Go to create, pattern, rectangular pattern. For type, select features and select the extruded
cut. For directions, click on the select box and
select the y-axis. For distance type, select spacing. Set the quantity and distance. Set the compute option to adjust. Let's remove this top body. As you hover over the body, it will be highlighted
in the bodies folder. Right click on the body and remove. Let's name the rings. It might also be a good idea to reorder the
bodies just to make the list of bodies more presentable. You can simply drag the bodies into position. This has no impact on the order of features
in the timeline. Let's hide all the rings and bring back the
triangular panel. We need to make this panel thicker through
an offset. Go to modify, offset face. Select the top face and set the offset distance
to 6. In order to create the tiered effect, we are
going to split this panel into 3 layers and shell each of these layers. Let's split out the top layer. Activate the surface tab. Go to create, offset. Select the top face and set the offset distance
to -2. This will create a surface body 2 mm underneath
the top face. It will serve as the cutting tool. Go to modify, split body. Select the solid body as the body to split. And select the surface body as the splitting
tool. When the surface body was created, you can
see that this edge is still submerged within the solid body. So we would need to extend the splitting tool
to ensure that it fully cuts through the solid. Let's rename and hide the first layer. Remove the surface body. We will repeat the process to split out a
second layer. So the triangular panel has been split into
3 layers. Let's hide the middle and bottom layers. Activate the solid tab. Go to modify, shell. Select these 2 faces and set the shell thickness. Hide the top layer and bring back the middle
layer for shelling. Lastly, shell the bottom layer. Let's bring back all 3 layers to take a look. Begin the fillet command. Select these 3 edges. Set the fillet radius. Go to the dialog box and click on this plus
sign to add another set. Add a third set. Next, we will be creating this step. Activate the surface tab. Go to create, offset. With the chain selection option checked, select
this face. Set an offset distance of -2. We are going to use this surface body to split
the top face. Go to modify, split face. Select the top face as the face to split. Select the surface body as the splitting tool. Extend the splitting tool. Let's remove the surface body. This is the resultant split face. Activate the solid tab. Go to modify, offset face. and raise this
surface by 2. So we have completed the triangular panel. Let's bring back the rings. Go to modify, combine and combine all these
bodies into one. Let's rename the resultant body and hide it
for the moment. Now, we shall create one of the bosses. First create a sketch on the top plane. Draw a circle of diameter 13. Align this horizontally with the origin. Start an extrude with this profile. Bring back the combined body from the previous
operation. And set the operation to join. Next, we need to create a counterbore. Let's use the hole command to do this. Select the top face. Drag the centerpoint of the hole and snap
it to the center of the boss. For extent, select all. For hole type, select counterbore. For hole tap type, select simple. For drill point, select flat. Adjust the counterbore dimensions. We want the top of the boss to follow this
curved face of the previous step that we created. We shall leverage on this existing face to
create a surface body for the cut. Activate the surface tab. Go to create, offset. Select the top face of the step. Set the offset distance to zero so that we
can create a copy of the face in the same location. Go to modify, split body and use the surface
body to split the boss. Extend the splitting tool. Lets remove both the excess body and the surface
body. We want to create another boss here using
the circular pattern command. For type, select features. Go to the timeline and select the boss extrude,
the counterbore and the split body features. Select the y-axis as the pattern axis. Instead of a full pattern, we will be going
for a partial pattern. For angular spacing, select angle and set
a total angle of 60. Set the quantity to 2. Set the compute option to identical. For some reason, this has created an empty
body. Let's remove that. Hide this body and bring back the hexagonal
panel. Looking at the final result, you can see that
the pattern does not extend all the way to the edge of the panel. There is a slight offset. Start a sketch on the top plane. Let's project the original hexagon by selecting
this face and pressing p. If we hide the body, we can see the projected
lines in purple. Create an offset sketch using these lines. Confirm the sketch and bring back the body. Go to modify, split body. We will split this hexagonal panel using the
offset sketch. Next, we shall create the seed or starting
hexagonal cut. Begin a sketch on the top plane. Center the hexagon on the origin. Adjust the number of sides and dimension. Add a vertical constraint to this edge. Draw a line from the origin to the midpoint
of this line. Draw another line from the origin to the midpoint
of the adjacent line. Set both of these lines to construction. These 2 lines will serve as directions during
the pattern. Create an extruded cut with this sketch. For extent type, select all. Go to create, pattern, rectangular pattern. For type, select features and select the extruded
cut. For directions, click on the select box. Bring back the sketch and select the 2 construction
lines. For distance type, select spacing. Adjust the quantity and distance. For direction type, set to symmetric for both. All 3 compute options will work. You can see that the pattern is restricted
to the inner body. This is because the first extruded cut only
went through the inner body. So even though we adjusted the pattern beyond
the inner body, the subsequent patterned cuts will only cut through the inner body. Let's combine these 2 bodies. Bring back the combined body consisting of
the ring and triangular panels. Begin a circular pattern. For type, select bodies and select this body. Select the y-axis as the pattern axis. Set the quantity to 3. Lastly, combine all these bodies into 1.
Sharp edges are bad for acoustics.
I've been workign with Fusion360 for years, but I still learned a ton from this video. Amazing and very well edited.
Some surprisingly good tips on there that I wish I leaned ages ago
Too busy for me, but I can appreciate the work and creativity that went into it