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Hey there, it’s Kevin Kennedy and welcome to this revised version of Day #2 of Learn Fusion 360 in 30 days. By the end of this tutorial, you’ll know how to 3D model a beer bottle. You’ll learn how to: insert a reference image, create a fit-point-spline, use the revolve feature, and add the appearance of glass.
To get started, if you’re following along with the 30-day series then you may want to create a new folder within the Learn Fusion 360 in 30 days project. To create a new folder, click the new folder button in the data panel. Then, label this folder “Day #2 – Beer Bottle.” Simply type that out in the input field and then hit the enter key on your keyboard to confirm the name change. Creating folders is a nice way to further organize your project files within the data panel.
You can also create a folder for “Day #1 – Lego”. Then, select the corresponding lego file with your mouse > right click on the file > and then select “move” from the list of available options. To move files around all you have to do is select which folder they should be moved to. Then, select that blue “Move” button to confirm the change.
Next, I’m going to hit the save icon in the upper lefthand corner of the toolbar. This will open up the save dialog box, in which I’ll type out “Beer Bottle” for the file name. Before clicking the save button, I’ll make sure the #2 folder is selected for the location settings. If it’s not selected, you can hit the caret icon to toggle open all of your folders…and then you can select the corresponding #2 folder, which ensures that the file will be placed there.
We’re now ready to insert our reference image, which we’ll use to draw the shape of the beer bottle. To download the reference image for this tutorial, head to my website at ProductDesignOnline.com/3…that’s ProductDesignOnline.com/3 and that URL will automatically redirect to the page with the resources for this tutorial.
Before I insert the image, I’m going to create a new component, which will nest all of the images, bodies, and other reference info in a nice component folder within the Fusion 360 browser.
To create a new component I’ll select the assemble dropdown list. Then, I’ll select “new component.” This opens up the new component dialog box, where we can type out a component name. I’ll type out “Beer Bottle” for the component name. Then, I’ll make sure empty component is selected, as we don’t currently have anything in our design. Lastly, I’ll make sure the “activate” box is checked, which activates our component as soon as we click the “OK” button. After double-checking those settings, I’ll click the “OK” button.
At this point, we can enter the reference image, which we’ll use as a guideline. We’re essentially going to trace over the image. The beer bottle is a fairly simple object, however, you’ll find reference images to be a great way to reverse engineer parts or designs – especially with more complex objects.
I’ll select the insert dropdown list and then I’ll select the “Attached Canvas” option. This opens up the “Attached Canvas” dialog box. You’ll see that the first option we need to define is the “face” that our reference image will be placed on. If we had other parts in our model then we could select a face of the model; however, we don’t have anything yet, so we’ll need to select one of the origin planes.
I’m going to select the XZ origin plane. Then, I’ll click on the “select image” icon, which opens up the file folders on your local machine. From here, I’ll select the image from my downloads folder and I’ll click the blue open button. You’ll notice the image is fairly small upon attaching it. To resize the image I’ll just click and hold the corner manipulator or the scaling icon, and I’m going to drag away from the image to make it larger. However, you’ll realize that this method is not very accurate. We’d rather have the exact dimensions of the image…so I’ll show you how to calibrate the image in just a minute.
First, I just want to point out that after we selected the image from the file folder, you may or may not have noticed that we have a number of additional options in the “Attached Canvas” dialog. We can now flip the image if needed… scale the image… change the opacity… along with a few other options.
For now, I’ll simply click the “OK” button so we can calibrate the size of the image. To calibrate the image we’ll have to right-click on the file in the canvases folder. As I mentioned at the beginning of this video, the component we created will group all of its relevant parts. Therefore, we’ll have to toggle open the “Beer Bottle” component… then we can toggle open the “Canvases” folder…and then you’ll see the image we attached. We can no right-click on the image to select the calibrate option.
The calibrate option lets us define two points on the image, and then we can define the distance between the two points. First, I’m going to hit the “Front” side of the viewcube in the upper right-hand corner to look directly at the image. Then, for the first point, I’ll click in the lower right-hand corner of the image. For the second point, I’ll click in the upper right-hand corner of the image.
You’ll notice immediately after placing the second point that the dimension input field opened up. Within the input field, I’ll type out 240mm. After typing out the dimension I’ll hit the enter key on my keyboard…and this time you’ll notice immediately after hitting the enter key that the image was scaled to the appropriate size. We’ll now be able to trace the image, creating our model at a 1 to 1 scale.
To start off the beer bottle I’m going to draw a line down the middle of the beer bottle. I’m only going to draw half of the image as I’ll show you how to use the “Revolve” command to create the entire 3-dimensional shape.
I’ll activate the line command with the keyboard shortcut letter “L,” as in Lima. Then, I’m going to click on the XZ origin plane as the plane to sketch on. I’ll click at the middle of the top of the bottle for the first point of the line…and I’ll click at the bottom of the bottle for the second point.
With the line command still active we’ll want to create the bottom of the bottle. Now the reference image I have used is at a slight perspective because the top and bottom of the beer bottle are not completely flat. To ensure that my bottle is flat, I’ll continue drawing lines by drawing a line straight to the right.
I’m going to type out 30mm for the length of the line. Then, I’m going to hit the tab key which locks the dimension in place. Locking the dimension ensures that we don’t accidentally change it as we move around our mouse cursor. At this point, I can click to set the line, where it snaps in at 90 degrees creating a horizontal line.
With the line command still active, I’ll draw a line heading towards the top. I’ll make this line 134mm, and then I’ll click to place the line. Then, I’m going to hit the escape key on my keyboard to clear all commands.
I’ll now want to use the fit-point-spline tool to create the curvature of the stem of the bottle. Before using the spline tool, I’m going to create some sketch points which will make the spline tool easier to use.
I’ll select the sketch dropdown list. Then, I’m going to select the “Point” command near the middle of the list. The point command simply lets us place sketch points every time we click with our mouse…and these sketch points can be used as reference points when we create other types of sketch geometry.
I’m going to zoom in on the stem of the bottle by using the center scroll wheel on my mouse…so it’s easier to work with the image. Then, I’ll simply click to place a number of sketch points at all of the points where I feel the curvature starts to change… ensuring that the points are spaced out as evenly as possible.
Once all the sketch points are in place, I’m going to activate the “Fit Point Spline” tool. I’ll select the sketch dropdown list and then I’ll find the spline flyout folder. You’ll see there’s a folder since there are two different types of splines. I’ll select the “Fit Point Spline” option from the list, which activates it.
Then, to draw the spline I’m going to click on the bottom sketch point and I’ll make my way towards the top clicking each sketch point one by one….
Once all of the sketch points are selected you can either hit the enter key on your keyboard, or you can select the checkmark icon that turns green as you hover over it with your mouse cursor. It’s important to note that you cannot hit the escape key right after creating your last spline point.
Although the escape key exits most commands after sketching out geometry…with the spline tool it will not only exit the command but it will also delete the recent spline geometry. This is something that I see beginners getting confused with all the time…so just be aware of this as you work with Fusion 360 splines.
After hitting enter or the checkmark we can then hit the escape key to make sure we don’t have the spline command still active. This will let us further define the beer bottles shape by dragging around the green manipulator handles of each spline point.
Really quick, I just want to point out that to create Fit Point Splines you don’t have to first create sketch points. You can simply click to place each point of the spline… however, I find that sketch points make it easier to create Fit Point Splines.
I’m just going to look at the spline and how it follows the reference image. If I see any of the areas to be off quite a bit, then I’ll simply click on the green spline handle points and I’ll drag them around until I’m happy with the overall shape.
To get the spline handles of one point to appear you can simply click on that one point… and to get the spline handles of all spline points to appear you can click on the entire spline.
You can also click and drag spline points to move them around… I’m going to double check that the top spline point lines up with the top of the first line that we drew. If it doesn’t, then I’ll simply click on the point and I’ll drag it around until they’re snapped to the same grid line.
Next, I’ll select the line command in the toolbar. I’m going to click to connect the endpoint of the left line and I’ll click again on the endpoint of the spline.
After connecting the two endpoints, you’ll notice our shape has become a closed profile, which is signified by this orange background highlight. This means we can use the profile shape with the revolve command, as it’s required that you have at least one closed profile.
I’m going to select the create dropdown list and then I’ll select the “Revolve” command from the list. Then, you’ll see that because we have only one profile Fusion 360 will automatically select it. If your profile isn’t selected then be sure to click on it to select it.
Next, we’ll have to select a revolve axis. I’ll select the axis selector in the dialog box and then I’m going to select the inside straight line of the beer bottle. You’ll see that we get a nice preview of the 3-dimensional shape that is being created by revolving the closed profile shape around the selected axis.
Additionally, you’ll see that in some scenarios you may need a revolve that isn’t 360 degrees or a fully symmetrical shape. If that is the case then you can update the degree field in the dialog box. For the beer bottle, we’ll simply leave this at 360 degrees and then I’ll click the “OK” button.
Now that we’ve created the overall beer bottle shape, we’ll need to finish it off by making it hollow and by rounding over some of its edges.
I’m going to first hit the keyboard shortcut letter “F,” as in Foxtrot, to activate the fillet command. We’ll use the fillet command to add a rounded edge to the bottom of this bottle.
I’ll select the bottom edge and then I’ll type out 5mm for the fillet radius. Then, before clicking the “OK” button, I’m going to add one more fillet to the top lip of the beer bottle. I’ll click the “Add new selection” plus symbol, which allows us to create multiple fillets with different radii, all within the same fillet command.
Then, I’m going to select the top edge of the beer bottle, and I’ll enter a fillet of just 1mm, as I don’t want this to have a sharp edge. Finally, I’ll click the “OK” button in the fillet dialog box to confirm the results.
To ensure the opening of the bottle is a set width, I’m going double-click on the sketch in the timeline, to open it back up. Then, I’m going to hit the keyboard shortcut letter “D,” as in Delta, to activate the sketch dimension tool. I’ll select the top line and I’ll add a dimension of 9mm.
Then, I’m going to right click on the line and I’ll select Horizontal/Vertical constraint. This constraint will ensure that the line stays horizontal. Don’t worry, I’ll be covering the topic of constraints further in depth later in this course.
Once that is complete I’ll hit the “stop sketch” button so we can make the bottle hollow.
To make the bottle hollow I’ll activate the shell command from the modify dropdown list…
Then, I’m going to select the body of the bottle by selecting the body in the Fusion 360 browser. I’ll type out 3mm for the thickness of the shell command, which is equal to the thickness we want the glass to be… and I’ll click the “OK” button to confirm the shell results.
At this point, we can’t tell if it’s hollow or not, as the top of our bottle is still sealed off. To look at the inside, we can use the section analysis tool. I’ll select the inspect dropdown menu…and then I’ll select the section analysis tool.
Next, I’m going to click on the XZ origin plane as the plane to view the model from. You’ll see this cuts our model in half, but only for the sake of viewing. Our full model is still there and we can turn this off at any time by clicking the section analysis lightbulb.
I’ll now hit the keyboard shortcut letter “C,” as in Charlie, to activate the center-circle command. Then, I’m going to select the top face of the bottle. We’re going to cut out a circle so the bottle has an opening. I’ll type out 14mm for the diameter and then I’ll hit the extrude icon in the toolbar.
In the Extrude dialog box, I’ll change the operation to “cut”. We’ll then want to set the extrude to cut to the other side of this top face. I’ll change the extent to the “to object” selection…and then I’ll select the bottom face. Finally, I’ll click “OK” to confirm the results.
Now that we have our hole cutout, we’ll need to add another fillet to this inner edge. I’m going to activate the model fillet command from the modify dropdown list. I’ll select the inner edge and I’ll add a fillet radius of 2mm, before clicking the “OK” button.
Then, I’ll be sure to turn off the section analysis by selecting its corresponding light bulb in the Fusion 360 browser.
To finish off the model lets add the appearance of glass.
First, I’m going to select the lightbulb next to the canvases folder, which turns off the reference image, as we no longer need it.
Then, I’m going to right-click anywhere in the canvas window, and I’ll select the appearance option.
This opens up the appearance dialog box, which hosts a number of premade appearances. They can then be dragged and dropped onto the model to make them look more realistic.
I’m going to search for glass in the search field. Then, I’ll scroll down until I see the “Glass (Bronze)” appearance. You’ll have to hit the download button to the right of the appearance, to download the appearance if you haven’t already done so. Then, I’m going to simply drag and drop the appearance onto the body of the bottle…and you’ll see that the glass appearance is now applied.
If you made it to the end of this video, then please let me know by commenting below if you found this revised version to be an improvement.
As always, I appreciate you taking the time to watch this tutorial. Please hit the thumbs up button below if you learned something in this video. Click on the video in the lower right-hand corner to watch the next video in this series.
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