3D Printable Pumpkin in Solidworks (Intermediate/Advanced Level)

In this Instructable I will show you how to properly model a pumpkin in Solidworks that can be 3d printed. I am a professional product designer and will share some of my modeling techniques here.

In creating the pumpkin’s shape, we will stay close to the anatomy of the pumpkin but we’re not aiming at a completely realistic representation. Instead, we will make it a bit more cute and friendly looking by simplifying some aspects. And instead of giving the pumpkin a face, I will show you how to create a pattern and text that will be partially cut out of the surface, so not all the way through. The reason for this is that we can put some small LED lights inside and when we turn them on, the pattern and text will become visible. The LED’s, a battery, and a switch will be embedded in a separate core part that can be removed from the pumpkin.

This is an intermediate/advanced level Instructable, so I expect you to already be familiar with SolidWorks’ basic modeling tools. I will not show you every little step but only the main approach. The modeling approach here is parametric, which means that you will be able to adjust most (ideally all) features (such as dimensions, amount of rind shells, shape of stem, depth of ribs etc.) even after the model is finished. This is the preferred way of modeling for more technology related professions such as industrial design, architecture and car design. It’s good practice to get used to this way of modeling – it may seem complex in the beginning and will require more thought and planning (which I have now done for you), but through practice you will progressively master it and become more used to it. With some dedication, the fruits of your labor will quickly show themselves!

To create one rind shell, we will first create the necessary sketches to derive the surfaces from. We start with the side profile sketch of the outer surface. Sketch this one on the right plane using a spline with only two spline points. Whatever you are modeling, you want to keep the spline points to a minimum.Create a smooth curve with the center spline point on the vertical axis and the outer spline point on the horizontal axis (coincident with the Top Plane). Create a ‘centerline’ tangent to the highest point of the curve so you can give a dimension to the height of the pumpkin. Then, make sure to mirror the curve about the horizontal axis. The main shape of the pumpkin will be identical on either side of the Top plane, but when we create complex surfaces in Solidworks we do need to create the entire surface first. So later we will cut the shape in half again, but for now we need to model the whole surface.

Now we need to decide how many rind shells the pumpkin will have. Most pumpkins have 10 but I decided on 8 for simplicity’s sake. We will now create a plane to draw the inner ‘rib’ of the pumpkin on, where the separate rind shells will come together. This plane will be derived from the right plane but at an angle. Therefore, you will also need to create a sketch with a vertical line through the origin, which will serve as the pumpkin’s center axis. The angle will depend on the amount of rind shells (rs) in the following way:  angle = 180/rs.

Now, create the section that defines the horizontal profile of the rind shell on the top plane. If you observe a pumpkin you will see that it is similar to the curve depicted in the image. Also create this curve preferably with only two spline points. The center point should be coincident with the first sketch’s midpoint, and the outer point should be coincident with the plane we just created. Then, mirror the curve about the centerline.

For the inner shell’s side profile sketch, offset the outer shell’s profile sketch by the amount specified as the minimum wall thickness of the material you would like to 3d print your pumpkin in. In my case, that is 0.8 mm. Then drag the spline points until they rest on the Y-axis.

Now draw the horizontal profile section on the Top plane. Connect it to the angled plane on one side and to the profile sketch you just created on the other side. In the center, the rind shell will have a minimum wall thickness so as much light as possible will pass through. For a nice gradient effect and to increase the strength of the construction, you can let the wall increase in thickness towards the sides.

Now you can draw the outer profile curve for the inner rind shell, where it connects to the next shell. Make sure to connect it to the two previous curves you drew, and to mirror it about the top plane. Then, create a sketch on the angled plane and do a ‘Convert Entities’ on both the inner and outer profile sketch for the rib. Connect the ends with straight vertical lines so you have a closed sketch. Then, create a planar surface from this sketch and mirror it about the Right plane. You should end up with your model looking like the one depicted in the image.

You will now create the double-curved surfaces for the rind shells. This is what will define the main shape of the pumpkin. We will use the Boundary surface technique. Select 3 curves in one direction: the outer rib profile sketch, the sketch for the outer side profile, and the rib profile on the other side, derived from the mirrored planar surface we just created. In the other direction, select the horizontal profile sketch. Make sure that the central sketches are in ‘Normal to Profile’ mode. SolidWorks will create a preview for you in which you can check the quality of the surface. Make sure it looks ok – it should display smooth curvature combs without negative values and fluent, continuous zebra stripes.

In the same way, create the inner surface of the rind shell. Then, knit the outer and inner shell surface together with the side planar surfaces, and check the option ‘Try to form solid’. This will give you the basic solid to build the pumpkin with. If this works out correctly for you, congratulations!

The pumpkin will have a cylinder through the core to contain the electronics. The diameter will depend on the battery you are using, in my case a CR2450 battery with a 24.50mm diameter. Adding 1mm on each side for the wall thickness makes for a diameter of 26.50mm for the core. You can create a circle with this size on the top plane with the center on the origin. Then, do an extruded cut to cut the cylinder out of the solid body you just created for the rind shell section.

One thing to mention here is to take into account small variations in the 3d print’s dimensions. This can be quite significant depending on the printing process used. I always leave 0.1-0.2mm extra free space around separate parts to prevent them from not fitting together.

What I will do here might seem a bit complicated, so bear with me. The intention is to create a pattern that we can cut out of the inside of the rind shell, to a depth that we can specify (so not all the way through). This pattern can be anything you like – geometrical shapes, stars, faces, letters, whatever. I have chosen for a diamond-type pattern. We are first going to draw this pattern on a plane, and then wrap it on to a cylinder. From there, we will project it onto a double-curved surface and from that surface we will project it finally onto the pumpkin. This is only one way to do it of course, but I find it preferable because I keep all the pattern data in a single sketch and can easily alter the way it will appear on the final surface.

First, create an offset of the inner rind surface. It should be offset about 0.5mm outwards, so your wall will not become too thin while the depth will still be significant enough for the pattern to be seen on the outside.

Now, create a cylinder from a circle sketch on the Right plane, to wrap your pattern sketch onto. Make sure that the cylinder is small enough to not cross the pumpkin’s surfaces. Also create a copy (offset 0mm) of the cylinder because we are going to use it again for projecting text onto one of the rind shells.

Now, create the pattern sketch on the Front plane and use the Wrap feature to wrap it over the cylinder.

Now, I want to project the wrapped elements onto a double curved surface, so that when I apply them onto the pumpkin they will also spread out horizontally. To create a double curved surface, first create a curve on the Right plane that is concentric with the cylinder. Then create a curve on the Top plane to define the horizontal spread of the pattern. A smaller radius will give rise to a larger spread. Use the ‘Swept surface’ feature to sweep the curves. Then you may have to mirror the surface across the Top plane. Make sure to check the ‘Knit surfaces’ option.

Now, create a new sketch on the Front plane and use ‘Convert entities’ for all the pattern elements wrapped onto the cylinder. Then, exit the sketch and project it onto the newly created swept surface. You can use ‘Delete face’ to delete the rest of the swept surface and be left only with the elements for the pattern.

Next, Use ‘Thicken’ on each individual element for the pattern to project it outwards, all the way through the solid body of the pumpkin’s rind shell. Make sure to untick ‘Merge result’, so you end up with a separate solid for each pattern element.
Before we erase the pattern bodies out of the main body, we want to create a copy of the main body so we can use it later for the piece that will contain the text. Use the ‘Move/Copy’ feature for this and specify a 0mm translation. Then hide the newly created body.

Now, use the earlier created offset surface to cut away the part of the pattern bodies that we are not going to subtract out of the main body. Use the ‘Cut with Surface’ feature and make sure the arrow is pointing outwards. Use the Combine – Subtract feature to eliminate all pattern bodies from the main body. Your pattern should now be neatly integrated into the pumpkin shell. If it succeeded, great job!

One simple trick you can use to simplify working with patterns and save you some mouse clicking as well as computing power is to simply apply the pattern on only a quarter of the rind shell, then cut away the other quarters with the Top and Right plane, and mirror the piece back together using the patterned body.

On one of the rind shells (the one we just made a copy of and did not apply the pattern onto) we are now going to create text in exactly the same way. It would be good exercise for you to try this yourself now, without much help. That’s why I’m only giving you a few tips:

- Use a baseline sketch to position the text
- Use the offset of the cylinder we created for a new ‘Wrap’ feature
- You may have to rotate the wrapped elements 180 degrees because the text may be facing the other way.
- Try to avoid very complicated fonts because it will take up a lot of memory
- Check the minimum detail level for your 3d printing process to determine the size of your font.

VERY IMPORTANT! After you have created the solid bodies for each letter, test if you can successfully subtract the text from the main body. If successful, delete the subtraction feature again! We will apply it again later in the process. For now, it is important that the letters are not yet subtracted from the main body.

Create a ‘Circular pattern’ to rotate all the rind shells around the central axis. Stick to the number of shells you decided on earlier (in my case eight). Beware that now your file may become very large and will take up a lot more working memory.

Delete the original shell with the pattern and instead of that one use the shell without the pattern that we will subtract the text from. Combine-Add all your rind shells into one body, and then do a ‘Cut with Surface’ to cut away the entire bottom half with the Top plane.

To blend the rind shells nicely together, you can use a ‘Variable radius fillet’ and play around with the values. You may then be able to do a ‘Circular pattern’ with this feature to apply it to all rind shells, but sometimes this doesn’t work and you will have to do all the fillets one by one.

We will now create a tube inside the pumpkin to house the core. For this, use the sketch originally used for the central vertical cylinder – the one you used to cut off the top and bottom parts of the rind shell. Extrude this sketch with the ‘Up to Body’ option up to the main body of the pumpkin, and give it a thickness outwards. This tube should have a decent thickness because we will apply some screw thread to it which might need to withstand some manual force.

Make the transition from the pumpkin’s main body to the tube more fluent with a 2-3mm fillet. Make sure to also fillet the inside edge to not lose too much wall thickness. Mirror the pumpkin body back together over the Top plane. Now finally, you can subtract the text from the rind shell.

Then , use the same sketch used to create the tube again to cut away the center part of the tube with an ‘Extruded Cut’ – since here the LED’s will have to be able to shine onto the outer surface. Specify two directions for the cut since at the bottom you need only a few millimeters while at the top you need about 10mm for the screw thread.

Then create the screw thread using a simple rectangular sketch on the Right plane and creating a helix curve with the ‘Helix/Spiral’ feature. The threading should not be thicker than 0.5mm. Then sweep the rectangle over the helix and combine the thread with the main body.

Using the flat horizontal surface at the bottom of the tube that holds the threading, create a sketch (circle) for the inner tube. This should fit right within the threading so it can pass through. Give it a gap of 0.1mm. Then create the inner tube by giving it a thickness inwards, and making it reach up to a vertex on the lower edge of the fillet you created on top of the pumpkin.

Then you can create the threading on the inner tube in the same fashion as you did on the outer tube. Make sure to leave a gap of at least 0.1mm for an optimal fit, and check if the inner threading matches the outer threading.

When this is done, cap the inner tube off by creating a sketch on its top surface. Do a ‘Convert entity’ on the sketch used for the inner tube, and then Extrude this one by a minimal amount.

To give the top a curved surface, we will use a ‘Dome’ feature. Give it a height of about 2.5mm and check ‘Elliptical dome’ to make the surface transition smoother.

You can now mirror this part about the Top plane and cut off the part containing the threading on the bottom section.

We are now ready to create the stem. On the front plane, draw the centerline for the stem. Then create a plane on each end of this curve by selecting the centerline and one of the end vertices. On this plane, sketch a circle on each end and then create a lofted surface using these two circles and the centerline. Make the upper circle a little bigger for a bit of an organic effect. Then blend the stem into the tube with a fillet, and finish the end of the stem with the Dome feature.

You can now connect the upper and lower part of the core part with a simple hollow tube, and create an inner structure in whatever way you like, depending on the components you are going to use in case you want to implement LED lights.

To make it ready for 3d printing, export the two parts separately to .STL format, and make sure to use an STL checker such as Netfabb or Magics to fix potential errors. My suggestion would be to print the main body in a white plastic, the core in a different color such as green, then use orange or amber LED lights and to put several of these around the house for a perfect Halloween atmosphere. 

Happy modeling, Happy 3d printing, and Happy Halloween!