Halloween pumpkin and tutorial

Here is one more Halloween pumpkin fidget. I added a (long) tutorial to let you design your own.

Please note that I use FreeCAD and the tutorial does too. I will try to explain as best as I can for you to design your own model with another CAD tool.

The shape

Note : you can create something other than a pumpkin shape, or start from some existing shape and skip this part. Do as you please.

The global shape is made by a revolution around the Z axis of "some shape", to which we add a few ridges to get a better pumpkin-looking result.

Design the outline of the pumpkin on a vertical plane (here, the XZ plane). I used a B-spline, you may go with whatever suits you aesthetically. Note that this sketch will also be used a few steps later to make the ridges along the body of the pumpkin.

This shape is used in a revolution around the Z axis. 

The result is closer to a squish ball than a pumpkin, it needs some ridges. This is done by a substractive pipe from a small shape (here, a triangle) along the outside of the shape. The path to follow is the B-spline from the first sketch, in grey hereunder.

The groove is a little bit harsh and un-natural looking, add some fillets on its sides. Then, perform a polar pattern of the ridge and fillet, around the Z axis. The number of occurrences (9 here) is the number of "slices" you want to get. This number is used several times thereafter, so better to define some variable for it.

Note : the fidget will be better looking with a even number of slices rather than odd one as shown here. With an odd number of slices, when fully deployed, the two bottom slices are at the same level ; with a even number of slices, there is one slice below the other, which I think is nicer.

The stem

What's a pumpkin without its stem ?

On the XY plane, offset in Z by the height of your shape, design the lower shape of the stem. I do a simple repeating arc around a circle but you may go with almost whater pleases you.

Pad this shape towards the inside of the pumpkin (a few mm are enough). This is done to fill the small spaces between the bottom ot the stem and the body of the pumpkin. Otherwise, the stem will only touch the skin of the pumpkin, and will very easily detach from it.

Somewhere above the previous sketch, draw the top of the stem. I keep the same design, only smaller. You may slant the sketch's plane, it will be better looking.

Draw some path that will be the center of the stem and will give it its global shape.

Perform an additive pipe of the base of the stem (the one that has already been padded towards the inside), following the path, and using the top of the stem as a transformation.

The shape is done !

Slicing the shape, straight cuts

No, it's not slicing as in PrusaSlicer yet. We still need to split our shape into several subshapes that will slide against each other. It's not as difficult as it may seem.

Note : in FreeCAD, by default, you cannot create a single body with multiple separate parts (which is the result of the slicing). There is an experimental setting, Allow compound, in the body's Data properties, to make this legit. Set it to Yes.

First, draw the cutting shape on the XY plane. It should be some long and very thin rectangle from the center of the model to the full half-width of the model, plus some just to be safe. On this rectangle you will add the sliding part, which must be self-locking between two adjacent slices (hence, a triangle here).

One VERY IMPORTANT note : do not be to shy about the width of the cutting shape. Depending on the printer and the filament, 0.2 mm may be too low : you will get a non-sliding pumpkin, with parts being (almost) fused together. On my printer, 0.3 is appropriate.

This cutting shape is used for a substractive pipe, up to somewhere above the model, so we need a driving path. A simple vertical line will be far enough.

Perform a substractive pipe of the cutting shape along the cutting driving path

If we stop here, after performing a polar transformation of the cutting pipe we won't get what we really want. The slices will slide against each other without limitation. Meaning they will fall on the floor (or the table, or your lap). We must add some internal locking mechanism for the slices to slide only up to some point in each direction.

Since the sliding path is fully vertical, that's easy. I will nonetheless follow a little more complex way, because all sliding paths are not vertical as we'll see in the next section.

First, we must add some inside box that will define the limits of the sliding. Create a sketch at mid-height of the model, above the XY plane. Using the cutting path sketch as a template, anchor a rectangle on the top of the inside sliding part.

Perform a symetrical pocket of this sketch. The height of this box will limit the movements of the slices of the pumpkin

We have the room for the lock, let's add it. As previously, create a sketch at mid-height and, still using the cutting path and the previous pocket as references, add another rectangle.

Beware of the clearance between the box and the lock edges. Do not go too low or they will fuse during printing. As shown above, the lock must go into the gliding part (or at least touch it).

Perform a symetrical padding of the lock. The maximum movement of the sliding parts will be half of (height of box - height of lock), so do not make too big a lock

And, last but not least, perform a polar transformation of the cutting shape, box and lock around the Z axis.

That's it ! Export into STL, slice, print and enjoy !

Slicing the shape, curving cuts

Vertically sliding parts give a nice fidget, but what about curving slices ?

Every step previously stay the same up to the cutting shape. What changes thereafter is the shape of the driving path (previously, a simple vertical line). We're now going for an helix around the Z axis.

So we have our cutting shape.

Instead of creating a substractive pipe, we create a substractive helix. But there is a trick here : we will need to add the box and lock to the model. Previously, the driving path being a stright line, it was very easy to put the box and lock sketch at the proper height and still connect them to the cutting shape.

No more here (at least with my limited FreeCAD mastery). We must attach the box sketch and the lock sketch to the cutting shape at some (almost) random height. Taking into account the fact that the cutting sketch follows an helix, this quickly gets weird.

So I cheat. Instead of having the cutting shape from the bottom to the top of the pumpkin, the sketch will be set at the model's half height. We are going to create two helixes, one going up, the other going down. The same is done for the box and the lock (which are already mi-height if you followed the previous section).

Please note we are going to create several helixes with the same main parameter (the helix pitch, which is the developped height of one turn of the helix). So write it down somewhere, or use a parametric variable for it.

Which pitch to choose ? You want a curving path, but not too much curving, something around 1/6 of a turn. Thus the pitch will be 6 times the main body height. Of course, if you want some really slanted sliding parts, lower the pitch. It should work, but I did not test it.

Give the helix some height, it must be higher than the pumpkin, stem included. In the following image, the height of the body is 50 mm, hence a 300 mm pitch (6x50) and a 50 mm height (remember, we start at half-height). And perform the substrative pipe.

For the second half of this first helix, we reuse the same sketch and make another substractive helix with the same pitch, but going down instead of up. We now have our first cut.

Since the plane of the cutting shape is set mid-height, it may be used as a reference to properly place the internal box and lock.

The box is carved out of the body, with the same helix parameters as for the cutting shape. Same stuff as previously : create a XY-parallel sketch mid-height and attach the box to the reference sketch of the cutting shape.

Then create a substractive helix going up (first half) and another one, from the same sketch, going down.

As can be seen, the box properly follows the cutting shape helix.

Then add the lock, exactly as above except it is an additive helix.

First create the sketch mid-height and attach the next-to-be box to the sliding part reference.

As said in the previous section, be careful of the clearances, do not go too low.

Then create an up-going helix and another down-going helix with this sketch, and the same parameters as all other helixes.

A close-up of the resulting helix stuff.

The last step is to perform a polar transformation of all the helixes.

And you are done

Export, slice and print. Happy Halloween !