- [Kevin] Hey there, I'm Kevin Kennedy, a product designer that helps
hobbyists learn Fusion 360. This free mini-course is
for absolute beginners, with no previous experience required. By the end of this tutorial, you'll have created your
very own customizable and 3D-printable stamps, with an interchangeable stamp plate. Learning Fusion 360 is a
critical step in being able to create your own unique
designs that you can 3D-print. Let's dive right in and get started! (upbeat music) Before modeling anything, I
like to name the design file. I'll click the Save icon in the upper left-hand
corner of the toolbar. This opens up the Save dialog box, in which you can choose the
name and location of the file. I'm going to type out "Kevin's
Custom Stamp" as the name. For the location, I'll hit the caret icon, which toggles open all
of the location settings. If you're brand new to Fusion 360, then you can create a new project by clicking the New Project button. I'll type out "Kevin Kennedy's
Class" for the project name. Then, you'll notice that you can also create folders
within each project. Folders are not required. However, they are simply a nice way to keep similar files
organized and grouped together. I'm going to make sure "Kevin
Kennedy's Class" is selected, and then I'll click the blue
Save button to save the file. Now that I've successfully
saved the design file, you'll see that the file name is now located within the file tab. We're now ready to start modeling. By the end of this course, you'll have created a custom stamp, which is made up of two different parts. The first part is the stamp
plate, which is interchangeable. And the second part is
the handle of the stamp, which can be re-used
with any stamping plate. As you create designs in Fusion 360, you'll want to create a new component for each and every part
that makes up your design. For this design, we'll create
one part for the handle, and one part for the reusable stamp plate. To create a new component, I'll select the assemble
dropdown list in the toolbar, then I'll select the New Component option. This opens up the New
Component dialog box. We currently don't have
anything in our file, so we'll have to use the default
Empty Component selection. Then, we'll want to name our component, so it's easier to find the
component in our model. I'll type out the word "Plate"
for the component name, then I'll click the OK button. Now the reason we have to create a new component for each part is that the component will group all of the relevant 2-dimensional sketches and other details of the part, which you'll see later on in this course. On the left-hand side of your Fusion 360, you'll see the Fusion 360 Browser. The browser can be viewed
as your file's structure. It will house all the different components or parts of your file, as well as the origin planes, and other objects that make up your part. You'll see that our plate
component is active, as signified by this
dot within the circle, next to the component name. We can now start creating
a 2-dimensional sketch, which we'll then be able to turn into a 3-dimensional object. At its core, our stamp
plate is simply a rectangle. And because we want the stamp
plate to be interchangeable, we're going to make it a
sliding dovetail joint. If you're not familiar, a
dovetail is a type of joint that is often used in woodworking. We'll make the sides
of our rectangle angled so it can slide in and out of the handle, without falling out. I'll activate the line command with the keyboard shortcut
letter "L", as in Lima. Once activated, you'll see that the three origin planes
are highlighted in orange. We'll have to select
one of the origin planes to draw the sketch on. These origin planes
correspond to the ViewCube, which is the cube in the
upper-right hand corner. You can click on the sides of the ViewCube to take a look at different
sides of your model or you can simply click and
drag the ViewCube around to look at the model from
all different angles. I'm going to click on the
front side of the ViewCube. Then, I'll click on the XZ origin plane. I can now draw lines on this XZ plane to create the 2D sketch that
represents the shape we want. I'll first click on the center origin, and I'll drag my mouse
cursor to the right. You'll then see a dimension
input field opens up. I'll type out 35 millimeters and then I'll click on
the red horizontal line to set the line in place. Next, I'll drag my mouse cursor up, and you'll see that we
can continue to draw lines as the line command is still active. I'll type out 70 degrees
for the angle input field, and then I'll hit the
Tab key on my keyboard, which locks the degrees into place. For the length dimension field,
I'll type out 5 millimeters, and I'll click on the left side, making sure the line going
back towards the origin point. For the next line, I'll create the angled
line on the left side. To do so, I'll hit the
Escape key on my keyboard which exits the line command. Then, I'll simply right-click
to select Repeat Line to quickly re-select it. I'll select the origin point. I'll type out 5 millimeters
for the dimension, followed by the Tab key to
lock the dimension in place. And once again, I'll type out 70 degrees for the degree input field, followed by the Tab key to
lock the degree in place. Then, I'll click to set the line in place. Lastly, I'll click on the other line to connect all the lines together, which creates a closed profile shape, as signified by the orange
background highlight. The key takeaway here is that you'll need a closed profile, or a fully-connected geometric shape, in order to use many
of the modeling tools. As you'll see in just a second, the modeling tools allow you to turn 2-dimensional sketches
into 3-dimensional shapes. In this case, we'll want to use the extrude command, which lets us add depth or thickness to a closed profile shape. I'll select the extrude command from the create dropdown list, located in the Solid tab. Once active, I'll select
the closed profile shape as the Extrude profile. I'll simply type out the dimension or length of this extrude. I'll type out 90 millimeters
in the distance input field, and then I'll click the OK
button to create the shape. We now have successfully created
our reusable stamp plate. To customize the stamp plate,
we'll be using your design that should be an SVG vector file. If you don't have an SVG file then you can use my sample file, which can be downloaded at
productdesignonline.com/16. That's productdesignonline.com/16. To insert the SVG, I'll select the Insert
dropdown list in the toolbar. Then, I'll select the Insert SVG option. Once the Insert SVG command is activated, you'll need to select a plane on which the SVG design
file will be placed. Of course, in this scenario, we want our design to
be on the stamp plate, so I'll select the top of the stamp plate. Immediately after selecting the
top face of the stamp plate, you'll notice the model was reoriented. For our convenience, Fusion 360 automatically changes the view so we're looking directly at it, making it easier to work with. Next, I'll click on the folder icon, located in the Insert SVG dialog box. This opens up the folders
on my computer's hard drive. From here, I'll select the Product
Design Online Stamp Demo file, and I'll click the Open button. After selecting the file, you'll notice that it's not
aligned with the stamp plate. To rotate the file I'll simply
click on the rotation slider and drag it over 90 degrees,
where it snaps into place. I'll also type out 2.5
millimeters for the Y-distance, in the Insert SVG dialog box, which moves the SVG file to the center. Now if you're using your own design file, then you can also drag the square to freely move the file around. Before we can click OK,
we'll have to take one of the most important steps. We need to hit the Horizontal Flip button in the dialog box, in order
to reverse our SVG image. We have to print our stamp out backward, so it's in the correct
orientation when we use it. Then, we can click OK. Above the ViewCube, you'll notice there are some
arrows show up on hover. You can use these arrows to
rotate the view of your model. I'll hit the right arrow so
I can look at this design from the correct orientation and I'll use the center
scroll wheel on my mouse, or you can use your laptop's trackpad, to zoom in closer to the design. At this point, we have 2D sketch lines that were created with the SVG file. We'll need to use the
extrude command once again, to turn the SVG into a
3-dimensional object. I'll activate the extrude command by hitting the keyboard
shortcut letter "E" as in echo. Then, I'll select all
of the closed profiles. In this case, this would
the outside border, the Product Design Online logo, and all of the letters, which I'll carefully select one-by-one. But first, if you're
enjoying the tutorial so far then go ahead and click that Like button, and be honest, if you're not enjoying it, then click that Dislike button. If you would like to
see a 3D printing series where I show you how to 3D model and 3D print common household items then comment, "3D" down below. If you happen to accidentally
select a profile, then simply click on it
again to deselect it. You can also click the "X" symbol in the dialog box, if you'd like to clear out all the
selections and start over. Once everything is selected, I'll type out 2 millimeters
for the distance, or thickness of the design. And finally, I'll click the OK button to confirm the extrude results. For a more freeform way
to look at your model, you can always use the Orbit tool, which is located at the
bottom of Fusion 360. Simply click the Orbit
tool on the far left, then click and hold in the canvas window to turn the model in any
direction you would like. Let's now take a look at
creating the stamp's handle. At this point, you've created
the reusable stamp plate, that now has either the sample file or your own unique design. To get started, we'll want to create a New
Component for the handle. As I mentioned at the
beginning of this course, you'll want to create a new component for each individual part of your design. I'll select the assemble dropdown list, then I'll select the New Component option. I'll name this component
"Handle" and then I'll click OK. If you now look at the Fusion 360 Browser, or file structure, on the left-hand side, you'll see that Handle component is nested within the plate component. And that's because I had
the plate component active while I created this new component. I actually want this handle
component to be nested on the same level as the plate component. To fix this, I'll click on
the Handle component name, and I'll drag it to the
top-level component, which is the file name. As I release my mouse on the file name, you'll see that the Handle
component moves slightly to the left, and it's now on the same
level as the plate component. As I mentioned earlier in the course, we're creating these components or parts, so they group our sketches and other design features
within each part name. You'll see under the plate
stamp I have two sketches and I have a bunch of Bodies which make up all the letters and the base of this stamp plate. I'll need to create the base of the handle that has a sliding dovetail
that matches the stamp plate. I want the base of the handle, to be centered with the stamp plate. To do this, I'll use one
of the construction planes, which lets us create sketches
in a more precise location. I'm going to select the
Construct dropdown list in the toolbar. Then, I'll select the Midplane
construction plane option. I'm selecting the midplane option because as the name suggests, it will let us create a plane in the middle of one of the parts. To create a midplane you'll have to select the two end
faces of the stamp plate. I'll select one side and then I'll use the ViewCube
to look at the other side. So I can select the second side. You'll see this positions, the orange construction
plane directly in the middle. Since everything looks correct, I'll click OK in the dialog box. Now that we have a plane
in the middle of our model, we'll want to recreate the dovetail shape for the base of the handle. However, instead of re-creating
it with the line command, we can save time by using
a tool called Project. I'll activate the project command with the keyboard shortcut
letter "P", as in papa. After activating the project tool, I'll click on the midplane
that I just created, as that's the plane I want
this new sketch to be on. Once again, Fusion 360
automatically reorients the view so it's easier for us
to work with the model. The project command lets
us simply select geometry in our model, and it converts it into 2-dimensional sketch
geometry on the plane that we have active. I'll need to select all four lines that make up the
silhouette of stamp plate. You can select them one-by-one, or you can also select within the shape, which selects all of the edges at once. I'll click OK in the project dialog box to confirm the results. If I now look at this
model from a slight angle, you'll see that the 4 lines
show up on the sketch plane. Notice the lines are purple, which signifies that the
lines were projected, or derived from the model's geometry. At this point, we'll want
to offset the trapezoid, so we can add a small tolerance
into the sliding dovetail, given that our final 3D printed object likely won't be perfect. I'll select the Offset
command from the toolbar in the Sketch contextual tab, because the offset command
lets us copy geometry, a specified distance away
from the selected geometry. Then, I'll select the
projected sketch geometry. For the offset dimension, I'll
type out 0.25 millimeters, which I've found works well
with my 3D printer after some trial and error testing. With that said, the
quality of your 3D print can vary based on many different factors, so you may find you'll have to adjust this after your first print. I'll then click the flip
button in the dialog box, to make sure the offset sketch is on the outside of the original sketch. Finally, I'll click the OK button to confirm the offset sketch geometry. Then, I'll right-click in order to select the
Repeat Offset option. I'm going to create a second offset in order to now create the thickness for the base of the handle. I'll select the original
sketch once again. Then, for this dimension
I'll type out 7 millimeters and once again, I'll flip it until it's on the outside
of the original sketch before clicking the OK button. We now have a closed profile
shape that we could extrude. However, we don't want the handle base to cover the stamp plate
or the stamp wouldn't work. To fix this, we'll need
to create some lines that run across the profile. I'll activate the Line tool by hitting the keyboard
shortcut letter "L" as in Lima. Then, I'll click on this inner corner and I'll draw the line
past the outside edge. I'll hit the Escape key on my keyboard to exit the line command. Then, I'll click on the
endpoint of the line and I'll drag it until it
snaps into the outside edge. I'll go ahead and repeat
this for the other side. I'll hit the keyboard shortcut
letter "L" as in Lima. I'll draw the line. Then, I'll hit the Escape
key and drag the line until it snaps into the outer line. Now you'll see I have
a closed profile shape that we can extrude to create
the base of the handle. Once again, I'll hit the keyboard shortcut
letter "E" as in echo, to activate the Extrude command. And I'll make sure the closed
profile shape is selected. This time, before typing out the distance, I'll change the Direction
option to the Symmetric option, which makes the extrude
distance go in both directions at the same time. For the distance, I'll
type out 25 millimeters, then I'll click the OK
button in the dialog box. We've now successfully created
the base of the handle. Let's finish off the handle by
creating some simple circles, which we'll then connect
together using the loft command. I'm going to use the ViewCube to look at the bottom of the model. Then, I'll hit the keyboard
shortcut letter "L" as in Lima, to activate the line tool. I'll click on the bottom
face of the model, as that's where I want to draw this line. Then, before drawing the line, I'll hit the construction
option in the sketch palette. Now the construction option lets you create sketch geometry that is used for reference purposes only. So they don't interfere with
any of the modeling commands. I'm going to then click on
the upper right-hand corner and then the lower left-hand corner, to create a diagonal line. Notice how this line is dashed, which represents that
it's a construction line. Next, I'll hit the keyboard
shortcut letter "C" as in Charlie, to activate
the center-circle tool. Before drawing the circle, I'll be sure to uncheck
the construction option in the sketch palette,
as we want this circle to be regular sketch geometry. I'll now hover my mouse cursor over the diagonal line near its center and I'll click to place the circle when I see the triangle
sketch constraint icon, which ensures the circle
we'll snap into place, directly in the middle of the line. So you should see a triangle icon. This is a good example of how you can use sketch geometry to help you further define
other pieces of geometry. I'll now drag out with my mouse and I'll type out 17 millimeters
for the circle's diameter. And then I'll hit the
Enter key on my keyboard. Before we can use the Loft
command to create the handle, we'll need a second piece of geometry, as the loft command requires at least two sketch
profiles or closed shapes. What I want to do is draw another circle. However, this one needs to be
60 millimeters above the one that I just created. Because Fusion 360 doesn't
let you simply draw in space, we'll need to create
another construction plane. This time, I'll click the Offset Plane
construction plane option, that's located in the Fusion 360 toolbar. Then, I'll click on the
surface that I just sketch on and I'll type out 60 millimeters
for the offset dimension. This will create the new plane, 60 millimeters from the selected plane. Finally, I'll click the OK
button to confirm the new plane. Once again, I'll hit the keyboard shortcut
letter "C" as in Charlie, to activate the center-circle tool. Then, I'll click the construction plane that I just created as
the plane to sketch on. I'll click on the center origin, then, I'll drag out with my cursor. I'll type out 30 millimeters
for this circle's diameter. And I'll click the
Enter key on my keyboard to set the circle in place. I can now use the Loft command to bridge these two shapes together. In simpler terms, you can
think of the Loft command as connecting the dots. I'll activate the Loft command from the create dropdown
list, in the Solid tab. I'll click on the small circle first, as we need to select the
closed profile shapes to Loft. Then, I'll click on the second circle. You'll now see how the Loft tool, bridges the two circles together. For now, I'll leave all the settings to the default settings and I'll click OK in the Loft dialog box. We could technically call
this handle finished, as it would be functional, however, let's add some rounded edges to the handle to make it
a bit more user-friendly. To create rounded edges, we'll need to use the Fillet command, which is located in the
modify dropdown list. In order to add rounded corners, I'll select the top edge of the handle. The Fillet command uses
a radius dimension, so I'll type out 10
millimeters for the radius or the distance from the
edge to the center point. Before clicking OK in
the fillet dialog box, I'll want to add one more fillet. If you want to add a
fillet of the same radius, then you can simply select more edges. However, if you want to
create another fillet with a different radius, you can click the plus symbol for the add new selection option. Next, I'll select the
bottom edge of the handle. For this fillet radius,
I'll type out 7 millimeters. Notice how this adds a
nice smooth transition because the base of the handle and the bottom of the handle
pole are joined together. Finally, I'll click OK in the dialog box to confirm the fillet results. To view the model in its entirety, we can right-click on
the top-level component or the file name and then select the Activate option. You can then use the
ViewCube or the Orbit tool, to take a look at your model. We've now successfully
created the stamp handle with a customizable stamp plate. Now that the stamp is finished, we're ready to export
the file for 3D printing. In order to 3D print this file, we'll need a .STL file, which is the most widely accepted format. To export as an .STL, I'll simply right-click
on the Plate component and then I'll select Save As STL. If you then click OK, you can save the STL file
to the desired location on your local machine. However, if you check the
option Send to 3D Print Utility, you can export the file directly to your 3D printer's slicing software. I use Ultimaker's Cura, so I'll select Cura
from the dropdown list. Then, I'll click the OK button. It's important to note, some of the available slicing softwares will not open up automatically. You'll have to open them up beforehand. You'll see the stamp plate design, successfully imported into Cura. I'll now do the same for the stamp handle. Back in Fusion 360, I'll right-click on the Handle component and then I'll select Save As STL. Now the handle prints best with the handle base
touching the build plate of the print bed. Therefore, I'll rotate the model around and this will differ based
on each slicing software so I'm not going to go
into specific details of how to rotate the model. Last but not least, it's important to note that you'll need to print
the handle with supports. The 3D-printed supports, that you'll break away after
the print is completed, are required for this gap that's
underneath the handle base. I've also found that this
stamp design prints best on some of the higher resolution settings that are available in slicing softwares... as you'll want the quality of the print to come out good enough that the stamp plate can
slide into the stamp handle, without too much friction. Remember, you can create
multiple stamp plates, in order to print out multiple designs. I suggest, simply clicking the File menu, selecting Save As, and then saving a copy of
the file as a different name. Then, you can use the timeline
at the bottom of Fusion 360 to go back and edit the design file. For example, I'll select the
second sketch in the timeline. Then, I'll hold down the Shift key and I'll select the
second extrude command, as both these features were used to create the stamp's design. Next, I'll right-click and
select the Delete option. Then, you'll want to make
sure your plate component is activated by clicking
the activate button to the right of the component name. At this point, you're able to insert another
SVG with a different design, to create more stamp plate designs. You can also use Fusion
360's native text feature if you simply just want to
spell out a name or word on your stamp. You'll then need to select the same stamp
plate face as before. Type out your desired word. Then adjust the settings accordingly. At this point, you'll
want to Extrude the text, just as we did with the SVG file in lesson or video number four. To summarize this course, I want to recap five of the
most important takeaways that you should remember. Number one. Always save your file with a file name before
beginning any design work. This ensures that your file will be saved should Fusion 360 ever crash. Number two. Always create
new components every time you're going to create a
new part in Fusion 360. This will keep all of your sketches and other features separate, which is essential as you build larger and more complex designs. Number three. Try to keep your sketches as simple as possible. As you saw in this course, each sketch should have a
limited amount of geometry. This makes sure they are
easy to update later on if you need to change
dimensions of your design. Number four. Create construction lines and geometry when you need geometry that is intended solely
for reference purposes. And finally, number five. Be creative. As you can see, in under an hour we've created this stamp
that can be customized to endless possibilities. Learning more about Fusion
360 will expand your knowledge and let you further customize
your own unique designs. In return, this could help
you gain more clients, make more money, and maximize
your creative potential. As always, I truly appreciate
you taking the time to watch this tutorial. Click that thumbs up icon if
you want more free content and click on that playlist in the lower right-hand corner to watch more 3D-printing
and Fusion 360 tutorials. To be a part of the Product
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