Twisted Succulent Planter


Introduction: Twisted Succulent Planter

About: Graduate student studying dynamics and control of elastic mechanisms. Background in Mechanical Engineering. 3D printing and CNC as a hobby.

This Instructable is an overview on the design process for a simple but elegant 3D printed succulent planter. It is designed with lots of drainage and a lower dish to collect the draining water. It is easy to slightly modify the dimensions and create a whole series of similar but distinctive planters. Mine are printed with PLA on a normal FDM 3D printer. The STL files for a large version (Main Image) and a small version are on thingiverse here

This is a reasonably detailed write-up on the design process aimed at someone who understands how to use basic sketch tools, boss extrudes, boss cuts but may not be experienced with lofting, shelling and more advanced sketching options (patterning, projecting, ect.).

I personally am using some small planter for my young propagations and a larger one for a mature spoon jade plant.

Step 1: Software

This process should work on any capable parametric CAD software such as Inventor, Fusion 360, Solidworks, PTC Creo. I originally designed this in Solidworks, but remade it in Fusion 360 for this Instructable. Fusion 360 is a capable modeling software where small start-ups and hobbyists can get a free license.

That being said, the Solidworks model I made was significantly easier to modify to adjust the design after. I found that the Fusion model broke if I adjusted many of my early sketches. If anyone with more experience in Fusion can explain how to avoid this issue I would appreciate it.

I do my slicing in Cura 3.3.1, but any slicer should work.

Step 2: Setup Top and Bottom Profiles

Here we need to setup a top profile and a bottom profile on two parallel planes. For this design both profiles are made up of 13 circular arcs.

The easy way to create a sketch with this radial symmetry is to first draw two equal length construction lines out from the origin and dimension the relative angle to be "360/N" where N is the number of segments you want. You can then draw a segment an arc between the two endpoints. To create the other 12 segments use the circular pattern tool.

Now the second profile is created in the exact same way as the first but on an offset plane. Create a new plane that is offset a fixed amount (60 mm here) from the plane the first sketch is on (probably top plane).

Step 3: Twisted Loft

The interesting feature of this design is all based on playing with parameters of the loft function. The basic idea of the loft is that we have two (or more) profiles that we want to fill between. This allows us to create complex geometry in a relative intuitive way.

When we select the two sketches as the loft profiles we get a pretty basic fill. This is pretty boring so we can use some of the other parameters to make it more fun.

First Tangency. We can modify the tangent properties of each profile to give us a more natural transition between the two. In Fusion this is the drop down that can change between "connected" and "direction." Change it to direction for the bottom profile. If your profiles are similar sizes the change will be subtle.

Second Twist. To make the profile twist we need to manipulate the loft handles. On each of the profiles you can see a set of white dots. These represent how one profile will map to the next. One by one drag all the handles on one of the profiles one arc over clockwise. You should now have the twisted profile.

Solidworks let you to specify only one handle and it guesses the other which normally works relatively well.

Mess around with the takeoff weight until you get a profile you like. Don't be afraid to go back and modify the dimensions on the profiles you made originally to make it look good. It is much easier to get the outer profile looking like you want it at this step instead of finishing and going all the way back.

Step 4: Shell and Drainage

Next create the cavity where the soil and plant will sit using the shell command. Select the face that we want the opening to be (the top in this case). It then allows your to change the wall thickness. I tend to use between 1.2 and 2.0 mm. You could probably go pretty thin with it if you have a nice, well tuned printer.

We are going to add two different types of holes in the bottom of the pot. First we will place three circular holes, again using the circular pattern to make them equally spaced. These are to help us locate and attach the water catch tray to the main pot.

Next we add in drainage. I chose to use 5 mm square holes. To fill the space we a rectangular pattern on the one square we have made. Adjust the spacing and quantity until they fill the entire space. Then you can uncheck all the individual instances that fall on or outside of the boarder.

Step 5: Drainage Standoffs

We will create the second component in the same design by making a second body.

Start with a sketch for the standoffs on the bottom face of the pot. Create two circles on it, a large one which will be the shoulder that the pot will sit on and a small one which will be the locating peg. The difference in diameter between the locating peg and hole in the pot is very important. The value you use depends on how well you have your printer dialed in among other things (such as print orientation). I used 0.25 mm overall diameter reduction but I would recommend starting larger and backing it down until you find what it takes to get a snap fit without breaking the part.

Use this sketch to extrude the standoff down. It is important to change the operation from "Merge" to "New Body" This will create three new bodies, one for each peg. Next use that same sketch to extrude the peg up through the bottom of the pot and down a little bit so that it will merge with the bodies we just created. If you have done this right you should have 4 bodies and when you select "body 1" you should see the planter highlighted blue and the pegs and standoffs still grey.

Step 6: Finish the Drainage Tray

To make the drainage tray seamlessly transition into the main pot we will use the project feature.

Create a sketch on the bottom of the standoffs. Select the "Project" operation and select the bottom face of the pot. Then offset that curve inward by your chosen wall thickness. We will use this sketch to create both the side walls and the bottom face of the drainage tray.

First extrude up the wall thickness selecting both areas in the drawing to create the bottom. Then extrude the wall up leaving an offset of between 1 and 2 mm between the bottom of the main planter and the top of the wall.

Step 7: Export, Slice and Print!

To get an STL file out of Fusion choose "Make" from the top menu, select the each of the two bodies one at a time and be sure to uncheck the "Send to 3D Print Utility."

Go ahead and slice and print the STL file however you personally prefer.

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