Create Your Own Customizable 3D-Printable Stamp in Fusion 360

SVG Demo File

Create Your Own SVG File

Using SVG Files with Fusion 360

Transcript

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!

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, that’s 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 easy to find the part or 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 video.

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 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 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-righthand 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 view cube around to look at your model from all 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 35mm 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 5mm, 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 to exit the line command. Then, I’ll right click and select “repeat line” to quickly re-select it. I’ll select the origin point. I’ll type out 5mm for the dimension, followed by the tab key to lock the dimension in place… and 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, creating 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 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 90mm 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.

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, 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 2.5mm for the Y-distance, in the “Insert SVG” dialog box, which moves the SVG file to the center. 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 okay, 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…

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 dialog box if you’d like to clear out all the selections.

Once everything is selected, I’ll type out 2mm for the distance, or thickness of the design. Finally, I’ll click the OK button to confirm the results.

For a more freeform way to look at your model, you can 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’d like.

Let’s now take a look at creating the stamp’s handle.

To get started, we’ll want to create a new component for the handle. As I mentioned at the beginning of the 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 underneath each part. 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.

In the next video lesson, I’m going to use the loft command to create the top part of the handle. But first, 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 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 0.25mm, 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 7mm…and once again, I’ll flip it to the outside 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 running 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. Keyboard shortcut letter “L,” as in Lima. Then, I’ll hit the escape key and drag the line until it snaps to 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 to the “Symmetric” option, which makes the extrude distance go in both directions at the same time.

For the distance, I’ll type out 25mm, 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. 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.

Now, I’ll hover my mouse cursor over the diagonal line near its center…and I’ll click when I see the triangle sketch constraint icon, which ensures the circle we’ll snap into place directly in the middle of the line. This is a good example of how you can use sketch construction geometry to help you further define other pieces of geometry.

I’ll now drag out with my mouse and I’ll type out 17mm 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 60mm 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 in the Fusion 360 toolbar.

Then, I’ll click on the surface that I just sketch on…and I’ll type out 60mm for the offset dimension. This will create the new plane 60mm from the selected plane. Finally, I’ll click OK 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 30mm for this circle’s diameter… and I’ll click the enter key 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 it 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 10mm for the radius or 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 7mm. Notice how this adds a nice smooth transition between the handle and stamp plate because the base of the handle and the bottom of the handle’s 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 and then select the “activate” option. Then, you can use the viewcube or the orbit tool, to move the model around.

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 [dot] .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 click the “Send to 3D Print Utility” option, 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 software will not open up automatically. You’ll have to open them 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.”

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 this 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 your slicing software…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.

In total, this should take about 2-3 hours to print out…but again, this will depend on your printer and the selected settings.

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 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 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 number four.

To summarize this course, I want to recap 5 of the most important takeaways that you should remember.

1. 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.
2. 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.
3. Try to keep your sketches as simple as possible. As you saw in this course, each sketch should have a limited amount of geometry on them. This makes sure they are easy to update later on if you need to change dimensions of your design.
4. Create “construction” lines and geometry when you need geometry that is intended solely for reference purposes.
5. 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.

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