Explore 3D

Part 3: Beginners Guide to Fusion 360

Blending & Sweeping

Johann Wyss

Issue 26, September 2019

This article includes additional downloadable resources.
Please log in to access.

Log in

In this installment of our Fusion 360 tutorial, we look at blending and sweeping.

This month, we'll look at the blending and sweeping functions in Fusion 360.

Understanding how to use these powerful tools can be very useful in CAD design. We will describe them separately to make learning them much more straightforward, compared to trying to combine them in one design.

Blending Your Objects:

Blending or more commonly referred to as loft (a testament to its origins in shipbuilding times) is the process of joining multiple two-dimensional drawings placed in parallel and spaced some distance apart into a single solid model. Generally, this function is used to create a transition from one shape to another.

As an example, let’s consider that we need to connect a 35mm diameter pipe to a 100mm x 20mm rectangular receiver. This could be a custom vacuum attachment to extract dust created with your CNC milling machine, or perhaps a duct needed to blow air across a heatsink. This would be very challenging to draw in CAD in a strictly 2D sense, thus the blend or loft function was born to calculate all the complex geometry needed to perform this task.

To get started, create a new project in Fusion 360.

Start by drawing the rectangle section. For our design, we want an internal structure of 100 x 20mm, and we want the part to have a 2mm thickness.

Press ‘R’ on your keyboard to enable the rectangle tool and draw two rectangles with the dimensions as shown above. This will form the initial shape that we will blend into a circular shape.

Note: Remember, we are parametric modelling, which means at any time you can go back and change the dimensions of a part. For example, you could adjust the internal dimensions of this rectangle and have the rest of the model recalculate the geometry to suit that change. This way, if something isn’t quite right, or you need the same part with a slight change, you do not need to redesign the entire part.

With the starting point of the transition drawn, we now need to add the final point. Since we want this part to fit over a 35mm diameter pipe we need a circle with a 35mm inner diameter. However, this transition needs a distance to complete the transition. 50mm should be more than sufficient to comfortably make this transition, while still being able to be 3D printed without any support material.

To add this distance, we need to create a plane that is parallel to the plane this drawing is on with a 50mm offset. This is done in the Construct menu. Click on the menu expand arrow of the construct button in the menu and select ‘Offset Plane’.

Select the plane to offset from, by clicking on its selection. Set the extent to distance and the distance to 50mm.

Now Press ‘C’ on your keyboard to enter the circle drawing tool and select the plane you just created as the origin. Starting at the origin point, you want to create the inner diameter of the circle to be 35mm. This is where the vacuum pipe will attach.

You may want to add a tolerance depending on how accurate your printer is. For this example, we will leave it at 35mm. We also want to keep the thickness to 2mm, therefore, we need to add 4mm to have an outside diameter 4mm greater than the inside diameter.

With both ends of the transition now sketched into CAD, we need to extrude them to create one solid model. To do this, we use the Loft tool. In the menu, select Loft from the Create menu.

With the loft tool enabled, select the two faces you want to combine, which creates a new body.

You should now have created a solid 3D object of that transition from a 104 x 24mm rectangle to a 39mm circle. We plan for our 3D print to be hollow, not solid, so we use the Shell tool to make it hollow. Select the bottom and top faces of the part you just created and choose the Shell from the Modify menu option.

With the top and bottom faces selected, set the inner thickness to 2mm.

Now we need to add an area for the vacuum pipe to attach to. Select the circular side of the model and press ‘C’ on your keyboard to enable the circle drawing tool. Using the origin point, create two circles, one the size of the outer dimension of the shape and another to match the dimension of the pipe this is going to go around. We set the internal dimension to 35mm (You may need to adjust your setting depending on the accuracy of your printer).

With the sketch you just created still highlighted, press ‘E’ on your keyboard to enter the Extrude function. We plan to extend this part by a distance of 25mm to connect our vacuum pipe, but you can do more or less depending on your application.

Repeat the same procedure to extend the rectangular end of your model. We chose a distance of 25mm. Adjust this setting to suit your purpose.

To provide a neater appearance, we add 0.5mm chamfers to both ends. In the Modify menu dropdown, select Chamfer and add the chamfers.

With your model complete, you can simply export it as a .stl file to print on your 3D printer. We printed our model on a Flashforge Creator Pro in Flashforge translucent PLA. At a 300-micron layer height, it took about 2.5 hours to print.


Let’s go one step further with the Blending technique by designing a small flower Vase with a subjectively aesthetically pleasing twisted shape.

To create this interesting shape, we create multiple polygon shapes of different sizes and offsets.

Using the Loft tool, start from the bottom polygon sketch up to the next sketch. To get the twisted shape, you need to drag the sketch loft points across to the next position. Once satisfied, finish the loft and move onto the next polygon.

With all the loft positions complete, you can simply Shell the object to create a hollow vase.

Using this technique can yield some very complex geometry that would not be easy to produce using any other means.

Common Fusion 360 Keyboard Shortcuts

CREDIT: autodesign.com/shortcuts/fusion-360

Sweeping Along A Path:

Sweeping is the process of having an extrusion follow an organic path. You first create the path in two dimensions across the x and y plane and then extrude a shape through it as a 3D object.

We most commonly use this function to create threads in our 3D designs. However, Fusion 360 now has many of the common thread sizes included in the thread function thankfully. This means you're only likely to to need to use sweeping for threads in Fusion 360 when making complex custom thread designs, which can become quite complex, so we will just keep things simple in this tutorial.

To teach you about this Sweep function, we will continue with the ducting example from our Blend tutorial.

We will show you how you can create a complex ducting solution that will follow a specific path. A common use for air ducting in our 3D printing hobby is for part cooling. Many printers do not come with part cooling fans, especially when building from a kit. These fans, whilst not necessary for functional prints, will greatly increase the finish and/or quality of your 3D printed objects. A part for a cooling fan is usually the first upgrade for kit 3D printers, so it makes sense that we create a 3D printable part cooling fan air duct.

To get started, you first want to design the path around the heatblock in Fusion 360. We’re using a Cocoon Create i3 printer in our example. but this i3 style of printer commonly have very similar sized components.

In our case, the printer’s heatblock is 20x20mm. Since this part gets very hot, we need a gap between this heatblock and the fan duct to prevent the air duct melting or softening from the high radiant heat. Let’s choose a minimum gap of 20mm.

We find the best way to design a part in this situation is to start drawing the known limitations into CAD itself. Since the build plate dimensions of our Flashforge Creator Pro are 220.50 x 145.50mm, this is a significant restriction, as is the heatblock size and minimum gap required. As such, we drew these limitations using the various drawing tools already discussed. This produced the sketch as shown above.

This sketch will greatly assist us in ensuring the design does not exceed the imposed printer limitations. Let’s now draw an arc 180° around this sketch with a radius of 90mm. Select Arc from the Sketch dropdown menu, and choose the ‘3-Point Arc’ option.

This is the path for our ducting so that it can comfortably flow over two or three sides of the part. Next, we want to create an extrusion that will extrude along this path. To do that, select Stop Sketch from the Sketch menu.

You now want to create a new drawing that you will extrude along that path we previously constructed. Since this will be 3D printed, the best shape for this will be a flat bottom and rounded top as this will not need an internal support structure.

Create the sketch as shown here, being sure to have the sketch centered to the path.

You can now use the Sweep tool to extrude that image across the path. Choose Sweep from the Create menu dropdown.

Note that this is a quite simple use of this Sweep function, just to get you started using it. Have a go at making some more complex shapes by simply changing the path. With practice, this will quickly become one of your favorite CAD tools.

You can now extrude the sketch along the path as shown here.

With the basic air path for our duct created using the Sweep tool, we can now proceed to complete the duct using other tools we have mentioned previously.

With the main ducting created, we now need a place to mount the fan. To do this, we need to create a centerline that goes from the origin point horizontally across the air duct. This line will help us build a fan mounting structure, which is central to the existing design.

Create a rectangle that is 55mm from the centre point, with dimensions of 24x17mm. These dimensions match the squirrel cage fan we plan to use, which has an output with the dimensions 20x15mm.

Extrude to a 12mm distance.

Use the Shell tool to hollow out the structure so that air can be flow through it.

Select both ends and the top surface of the fan mounting structure to have them as openings. We will close the two main ends later.

You now want to draw and extrude the exact shape needed for your fan to mount into the duct. In our case, 20x15mm. This will extend the shape as shown, leaving the internal gap for the fan to slot into.

We now need to close the ends of the duct as we want the air to be blowing toward the centre of the duct.Do this using the Revolve tool, which we explained in Issue 25. Select one of the exposed ends to start a sketch from it. You want to replicate half of the sketch so that we can revolve it around a centreline 180° and close this shape off. Using the Line and Arc tool, trace around half of the shape as shown and create a centerline to use as our axis.

You can now use the Revolve tool to close this end off as shown here.

Repeat the same procedure for the other side so that both ends are fully closed off.

With both ends closed, you next create some openings so that air can be forced out and over the part you’re 3D printing. To do this, simply make one sketch and extrusion that we repeat using the Pattern tool we discussed in Issue 25. We did this by creating a 4x4mm square, which we extruded as a symmetrical 2.5mm cut, as shown here.

We can now use the Pattern tool to repeat this cut six more times across this face, which provides all of the required vents.

Finish the design by adding chamfers, which will enable the part to print well and generally improve the overall appearance. We chose a 1mm chamfer on the lower surfaces and a 2mm chamfer on the vents on top to help direct air downward. We also added some 2mm fillets to the fan mounting structure.

Note: If you wish to use this part, you’re going to need to finish designing the mounting structure specific to your brand of 3D printer. This tutorial gives you a good head start, or at least an idea, of how you can easily and quickly create a part cooling fan for your printer in Fusion 360.

We have printed our design as is so you can see the final result. You can decide if its design is suitable for your specific application.

Output the .stl print file by going to the Make button in the main menu, which you can slice and print on your 3D printer.

Our model was printed on our Flashforge Creator Pro using Flashforge olive PLA. At a 200-micron layer height, it took 1.5 hours to print.

We noticed that the 25mm minimum clearance on our print was larger than was required. The beauty of parametric modeling is that we can easily adjust the size using the timeline on the bottom left of the screen.