SOLIDWORKS Magic Up in the Sky: Building Parade Balloons

As we wind down from the fantastic Thanksgiving parade that happened last Thursday, now is a great time to reflect on the preparation and engineering that goes into making those parade balloons soar! The first instance of parade balloons being used was back in 1927. This is where Felix the Cat made his first-ever appearance. Here, in SOLIDWORKS, I have modeled a similar looking balloon to inspect its design.

Felix Inspired Parade Balloon in SOLIDWORKS 3D CAD Software

The construction is fairly simple, being combinations of spheres, cylinders, cones and capsules. In the original photo, I used the height of the clowns to make an educated guess as to the approximate size of the balloon.

After scaling one of the feet appropriately, I use the new 2018 feature to create a bounding box. After doing so, I can easily determine that the length was 55 feet with a width of 23 feet and a height of 36 feet. This is reasonable, considering the dimensions of known parade balloons. Before I shell this out to find the mass of the rubber, I will head to mass properties to see the volume of the cat. This helps me see how much air we need, neglecting the thickness of the rubber.

Mass Properties Image in SOLIDWORKS

Here we can see that the volume (of helium/air required) is around 10,700 cubic feet. We can also see how much material we need by noting the surface area of the model, which is about 3,600 square feet. In this case, we can ignore the mass (of over half a million pounds) because these mass property calculations assume that this model is solid rubber — which is certainly not the case! If we want to see the mass of the rubber, we have to shell the model.

Shelling our Flex Inspired Balloon Model

When shelling the model (assuming a thickness of 0.018in) we see that the mass of the uninflated balloon is much more reasonable, clocking in at 350 pounds. Note the doubling of the surface area due to the inner surfaces being counted. Now that we have answered the question of how much material we need overall, another question arises in its place. How much material do we need per item?

The questions of how much material every patch needs AND what shape needs to be cut out in a flat pattern are tricky to answer today, and they certainly were for the engineers back in 1927. Luckily the design is just a bunch of cones, spheres and cylinders put together; hand calculation of these patterns is feasible. While that may work for our feline friend, it will not for our beagle buddy, as described in the next section.

Over the years, the Macy’s Thanksgiving Day parade has seen tons of iconic balloons march through the streets. One of the most iconic is this guy. You’ll see my Snoopy-inspired parade balloon modeled below in SOLIDWORKS:

Snoopy Inspired Parade Balloon in SOLIDWORKS

Thankfully, much of the analysis is easily done by SOLIDWORKS. When this balloon is 60 feet long from foot to nose, the volume of helium/air required to fill him is 11,500 cubic feet of air, the surface area is 4,200 square feet and the mass of the uninflated polyurethane balloon is 590 pounds. We find ourselves with the same task as constructing the cat: What shape does each piece need to be?

We can no longer assume that each piece is analytical geometry … is all hope lost? Not at all! With SOLIDWORKS, we carry the weight of this task with ease! We will use a feature that comes with every seat of SOLIDWORKS Premium: Surface Flatten.

Surface Flatten is found under the Surfaces tab of the command manager. SOLIDWORKS can flatten any surface, analytical or developable, with internal holes or without. It can also flatten curves, sketches and edges on the surface. Relief cuts can also be included with sketches, although we will assume the polyurethane/rubber is stretchy enough for our purposes.

But enough of the introduction. Let’s get to flattening! In the first blue box, we select the faces that we want to flatten. In the second pink box, we select a reference entity to flatten from. This can be an edge, but here, I pick a vertex on top of the head. We would populate the third green box if he had sketch entities on the surface that need to be flattened as well, but in this case, we do not. If we also needed to rip the flattened surface, we can specify this as well, but in this case, it’s not needed. Lastly, there is an accuracy slider. Since we are mapping curved surfaces to flat planes, there will be a factor of error involved. We can control how much error is introduced by playing around with this slider. Keep in mind that higher accuracy will lead to longer rebuild times. Below is the Property Manager of the tool as well as our preview.

Property Manager Tool Using Snoopy Inspired SOLIDWORKS Parade Balloon

When we hit ok, the result is generated as a new surface body tangent to the original selection at the flatten point (shown in gray). By looking at how the smile has stretched out, we can see there was quite a bit of deformation. Is there a way to find out how much? By right clicking on the flatten body, there is an option for a deformation plot.

Flatten Body

From the plot’s legend, we see that the surface experiences anywhere from 10% compression all the way to 18% stretch during flattening. That’s a little much, even for stretchy materials like polyurethane. Will this balloon ever fly? Well, we can try to have more pieces that we eventually stitch together to reduce this stretch. I have the head split into three faces per side. Let’s see what happens when we flatten each individually.

Flatten Individual Pieces

It’s already looking so much better, but let the numbers speak for themselves. Checking each surface, we see that the deformation reads anywhere from 1.5% compression to 1.5% stretch, which is acceptable. If the new results were not sufficient, we could always split the faces even further with split line!

Now that we have a nice flat pattern, how do we get it to the manufacturer? Just like sheet metal parts and other flat faces, we can export these to DXF easily by right-clicking the face(s) and selecting Export to DXF.

Export to DXF

Just like that, we can now send this out to the manufacturer. We can even apply it to our cat companion at the beginning of this blog.

DXF Felix Inspired Balloon from SOLIDWORKS

Here we have the ever-keen eyes of our cat and his mouth. So as we enjoyed the Macy’s Thanksgiving Day parade with our families, I hope you liked this look into how these balloons are brought to life by the engineers.

Author: Robert Maldonado, Application Engineer at DesignPoint

DesignPoint is passionate about building solutions that help product design, engineering and manufacturing companies maximize their potential. By developing trusted partnerships, we help our customers achieve game-changing results and support them in their journey as they strive for more. With DesignPoint, More is Possible.® Our solutions include SOLIDWORKS 3D software, 3D Systems and MarkForged 3D printers, technical support, training and more. Contact us today at!