A week ago I received an email from Jose Diaz with the question how to model a Dodecahedron in SolidWorks. I didn’t even know what a Dodecahedron was… Wikipedia says the following about it: “In geometry, a dodecahedron is any polyhedron with twelve flat faces, but usually a regular dodecahedron is meant: a Platonic solid. It is composed of 12 regular pentagonal faces, with three [...]
A week ago I received an email from Jose Diaz with the question how to model a Dodecahedron in SolidWorks. I didn’t even know what a Dodecahedron was…
Wikipedia says the following about it:
“In geometry, a dodecahedron is any polyhedron with twelve flat faces, but usually a regular dodecahedron is meant: a Platonic solid. It is composed of 12 regular pentagonal faces, with three meeting at each vertex, and is represented by the Schläfli symbol {5,3}. It has 20 vertices, 30 edges and 160 diagonals.” – Wikipedia
After a little research I discovered a SolidWorks model of Azrael from Grabcad. His SolidWorks model is so interesting that I’ve written a tutorial about it. Below I will show you exactly how to model a Dodecahedron with only two features in SolidWorks! I will also teach you how to use the Equations feature. Enjoy it and don’t forget to share this tutorial with other SolidWorkers!
Open a new part with model units set to millimeters
Go to: File > New > Part 
Create a 2D sketch
Select the Top Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon 
The display changes so the Top plane faces you.
Create a Construction Circle
Go to Tools > Sketch Entities > Circle or click at the circle icon 
Create a sketch which starts at the Origin. 
Change the dimensions of the circle into 100 mm by clicking at the dimension button 
Click at the Circle and change the Solid Line into a Centerline by clicking at the For Construction option
Click OK 
Draw a Polygon
Go toTools > Sketch Entities > Polygon or click at the polygon icon 
Change the number of corners into 5 as shown in the picture
Make sure that the top point of the Polygon is connected with the construction circle
Select the top point of the polygon, hold down the Control key and select the circle
Click at the Coincident relation feature to add a relation between the polygon and circle 
Make the sketch fully defined as shown in the picture
There has to be a Ratio between the dimension of the Polygon and the height of the Extrude
For a Dodecahedron this ratio is 1 : Sinus( 18)+1.
When the dimension of the circle is 100, the height of the Extrude has to be Height Extrude x Sin(18)+1
With the Equations feature you can automate complicated relations between the size of the construction circle and the height of the Extrude.
Let’s add the Equations for this model.
Go to Tools > Equations or click at the Equations button 
Go to Add
Type: “Ratio”=sin(18)+1
Click OK
Now SolidWorks knows what the value of the “Ratio” is.
Add a second Equations
The Height of the Dodecahedron has to be the Ratio x the dimension of Sketch1
Go to Add
Type: “Height”= “D1@Sketch1″ * “Ratio”
NOTE: For “D1@Sketch1″ you can click at the dimension of Sketch1 instead of writing “D1@Sketch1”
Click OK
Now SolidWorks knows that the “Height” of the Dodecahedron is the Dimension of Sketch1 x the Ratio.
Click OK
Create an Extruded Boss/Base
Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 
The Boss-Extrude menu appears
Direction 1 is set to Blind 
Change D1 into 10 mm 
Click at the Draft icon 
Change the Angle into 26.56505118deg
Select the Draft outward option
Click OK
SolidWorks has to know that the “Height” is equal to the height (D1) of Extrude1.
Add a third Equation for this model.
Go to Tools > Equations or click at the Equations button
Type: “D1@Boss-Extrude1″ = “Height”
Click OK
As you can see in the picture, the height of the Extrude changes into 130.9mm.
(if not click at the Rebuild button ) 
Create another 2D sketch
Select the blue surface and create a sketch by clicking on the 2D Sketch icon
Click at the Normal To button to look perpendicular on the blue surface 
Change the view into a Wireframe
Click at the Hidden Line Visible box in the ViewManager 
Create a Construction Circle
Go to Tools > Sketch Entities > Circle or click at the circle icon
Create a sketch which starts at the Origin.
Connect the circle with a point of the previous polygon as shown in the picture
Click at the Circle and change the Solid Line into a Centerline by clicking at the For Construction option
Click OK
Draw a Polygon
Go to Tools > Sketch Entities > Polygon or click at the polygon icon
Change the number of corners into 5 as shown in the picture.
Place the new Polygon exactly between the previous polygon as shown in the pictures
Use construction lines when necessary.
Create an Extruded Cut
Go to: Insert > Cut > Extrude or click at the Extrude Cut icon 
The Cut-Extrude menu appears
Direction 1 is set to Blind
Change D1 into 10 mm
Click at the Draft icon
Change the Angle into 26.56505118deg
Select the Flip side to cut
Click OK
SolidWorks has to know that the height of the Cut Extrude is equal to the height (D1) of Extrude1.
Add a fourth Equation for this model.
Go to Tools > Equations or click at the Equations button
Type: “D1@Cut-Extrude1″ = “Height”
Click OK
As you can see in the picture, the height of the Extrude changes into 130.9mm.
(if not click at the Rebuild button )
Well that’s all! You’ve just created a perfect Dodecahedron and hopefully learned something about the Equations feature. And the best part is, when you change the size of the first polygon sketch, the sizes of all the other features will automatically change as well (thanks to the Equations).
If you’ve, just like José, a specific modeling question about SolidWorks, let me know and perhaps I will write a tutorial about it.
Feel free to leave a comment or question below!
Click here to download the SolidWorks file of my Dodecahedron
15 Responses
You’re just amazing many are the things that were a nightmare to me but because of your teachings I have come up to be somewhere especially in our country where solidworks is still new in the world of engineering. Currently, we are less than 20 peaple who understands it countrywide.
be blessed brother.
Good Tutorial, Jan-Willem Zuyderduyn
This is very Useful And short method to make such profiles.
I have also made the same model With a different method. http://grabcad.com/library/request-dodechahedron
As well as i have created a tutorial for the same. http://grabcad.com/questions/tutorial-how-to-make-dodechahedron–1
Just because that’s what we do (isn’t it?), I decided to see if I could come up with a dirtier way to do it, using patterning, though your’s is definitely more elegant.
Here’s what I came up with:
1. Extrude a pentagon. You could make this more elegant by calculating how high off the origin plane you want to make it, and avoid a few steps by using that plane later, but remember this is supposed to be dirty.
2. Grab one of the ‘top’ edges of your hex, and the ‘top’ face of your hex, and create a plane . Here, I didn’t figure out a good ‘dirty’ way to compensate. You have to know that the angle between faces is approx 116.5650512. So the angle of your plane will be (360-116.5650512)/2 = 121.7174744 [thanks internetz for that angle].
3. Mirror your hex about that face.
4. You now have 2 pentagons, joined at one edge. Take your second pentagon, and rotate it about an axis normal to the center of your first 5 times in 360 degrees, using a circular pattern.
You now have the top half of your shape.
5. More dirtiness. You need to find where to put the center plane for your Dodecahedron. The ‘top’ of each of your pentagons is going to be your final surface, so grab the top edge of 3 of the bottom points (where it will protrude into the bottom half) in your circular pattern of hexes and make a plane. Then grab 3 points at the top edge (where the bottom half will protrude into the top half) of the ragged part, and create another plane. Using these two planes, make a plane between them. This is the center plane of the Dodecahedron.
6. Mirror the whole thing about this center plane, but don’t merge the two parts (uncheck the merge box).
7. Using Insert -> Feature -> Move/Copy rotate your bottom half 36 degrees (360/5/2 – or one half rotation you used to create the circular pattern in the top half).
8. Use Insert-> Features -> Join to join your 2 halves.
Voila – you have a Dodecahedron that you can make any size. If you made the original extrude thick enough, it will be solid. Else, it will be hollow. And all you needed to know in advance was that one angle between sides.
thanks! please write more free tutorials for us! specially about product design…
Your Comments
It looks like my Equation table is completely different – I am using SW 2012 SP5 & SW 2013 SP0
I liked Jan-Willem’s “boss-extrude-up / extruded-cut-down” technique, but wanted to do it without relying on Wiki for the mathematical formulas. Here is my “no trig” method. I have 2012 Professional.
A. Add a Global Variable “SideLength” = 100 (I work in mm and this can be later changed to whatever size you want.)
B. Create a 2D sketch on the Top plane. Insert a 5-sided polygon, centered on the origin. Put the “point” up and make the bottom side Horizontal. Dimension it to = the global variable “SideLength”. Sketch is now fully defined. Add a construction line between the left & right points. (This will be the “horizontal width” reference.) Add another construction line between the top point and the midpoint of the bottom edge (“vertical width” reference). Name the sketch “Bottom”.
C. Now I need to determine the extrude angle and the extrude height.
Start a 3D Sketch and, starting at the bottom line of the 2D sketch, draw 4 solid lines and 2 construction lines (to match the first polygon).
To get these lines on a plane, select the midpoint of the horizontal construction line and make it coincident with the vertical construction line. Make the horizontal line = same line in 2D sketch and parallel to the bottom side. Set the 4 solid lines = base line. We now have one side polygon that is the right size, but at an unknown angle.
D. In the same 3D sketch, draw a second polygon attached to the left of the first one by using 3 solid lines and 2 construction lines. Make the horizontal construction line midpoint to the vertical one and = to the 2D one’s length and parallel to the base line. Make the 3 solid lines = base line. You now have a fully defined 3D sketch.
E. Add 3 driven dimensions to the 3D sketch. Needed for Global Variables.
Angle between vertical line of 2D sketch and first side of 3D sketch. Rename this dimension “Wall Angle” (about 116.6 degrees).
Vertical length from Top plane to top point of first side (about 137.6 mm). Rename this “Upper Side”.
Vertical length from Top plane too lower vertex point of first side (about 85.1 mm). Rename this “Lower Side”.
Save the 3D Sketch, then open it again.
F. Now we can add the Global Variables we need for the Features.
SideAngle = (click on the “Wall Angle” dimension) – 90 (Evaluates to 26.6 degress)
OverallHeight = (click on the “Upper Side” dimension) + (click on the “Lower Side” dimension) (Evaluates to 222.7 mm)
Close the 3D sketch.
G. Boss Extrude using the Bottom sketch. Draft outwards. Use the defaults for distance and extrude angle and save.
Double click on the feature to show the dimensions. Double click on the blue dots and change the Depth to = “OverallHeight” and the Angle to = “SideAngle”. Rebuild.
H. Create 2D sketch on top surface. Add a 5-sided polygon at the origin with the “point” down. Make the top line horizontal and dimension it to = “SideLength”. Save sketch as “Top”.
G. Cut Extrude using Top sketch. Flip Side to Cut. Draft Angle. Use the defaults.
Double click on the feature to show the dimensions. Double click on the blue dots and change the Depth to = “OverallHeight” and the Angle to = “SideAngle”. Rebuild.
That’s it. As a wise man once said, “There are many ways to skin a cat . . . and they’re all good.”
hi jan
i want to know have can i use surface for design a tepot. i will be appropriated you help me in this kinds of design.
best regards
reza
I think that there is a much simpler option that does not rely on having to measure any angles.
For the dodecahedron.
1. On the top plane draw a pentagon centred on the origin with a set length for one edge.
2. Make a planar surface
3. Create a 3D Sketch.
4. Draw a line between two non-neighbouring points of the pentagon, and two further lines to create a triangle. Dimension the angles to 60 degrees. or make equilateral with equal sketch relations.
5. draw one additional line from the top of the triangle down to the point of the pentagon that is mid-way between the base of the triangle.
6. Dimension this to be equal to the edge of the original pentagon size.
7. Create a new reference plane using the top point of the 3D sketch and two points of the base.
8. Sketch on the new plane a pentagon and add relations to lock the corners together.
9. Planer surface.
10. Create an axis using the front and right planes.
11. Pattern second surface body 5 times
12. knit surfaces.
13. Now we need to create a second axis by using two points. Select two mid points from the edges of the body.
14. Circular pattern the body about the axis.
15. Knit (try to form solid)
No angles required
Nicely done, but two comments:
When you set the size in the first sketch, I would place it into the equation manager. That way it becomes a convenient place to control all of the variables.
Next, in the extrude cut, I used an up to next end condition instead of a fixed blind value. Just seems to be more flexible.
If we want to have fun, the next step is to convert the solid to sheet metal. make the bends and rips, unsuppress the flat pattern, print, cut and fold. Print out an image of the rendered part and the flat pattern. Now just place it on your desk as a conversation piece.
Jan, I like your work – I have followed it for a while. I like this thread, it has produced some good discussion – I will add to it (hope you don’t mind).
I have tried; to see if I could and to see if it would be reliable (it seems to be?) – produce the same shape as a single part from a wire frame! The wire frame is a single 3d sketch – took some effort. The model is then surface loft (x4) a pattern and knit to solid.
The base feature is an inscribed sphere – the only dimension to alter – it gives the size across flats, the rest of the model is driven by relations in the 3d sketch.
Enjoy – I did. Thanks.
Have a look…..
http://grabcad.com/library/dodecahedron-from-wire-frame/files
thank you sir………….
then
how to draw a helical gear, bevel gear and more gears………..
Just as Julian, I tried it the wireframe way.
There is only a 3D sketch for the “wire envelope” and only TWO dimensions: one variable, for the edge length and 108 degrees for the angle between two edges connected at the same vertice.
Start with a pentagon and make all five points ON PLANE (top one). Selec all lines and make them equal then add a dimension to make it fully defined.
After that, start drawing the edges and dimension the two 108 angles for each one, to define the direction. Once you add the EQUAL relation the new edge is fully defined.
Work your way “up” until you define the whole frame.
That’s a very nice approach Julian. I always like to have the geometry do as much of the work as possible.
I’ve found this to be an entertaining post, mainly because I’m probably one of the very few people that has ever actually NEEDED to draw a dodecahedron! I can say in 24 years of CAD I’ve never had much need for platonic solids, however a friend was making die for a game. I extruded a pentagon, then assembled the sides, constraining edges to each other. I had hoped to come up with a pure/mathematical solution but this was quick and practical. In just a few minutes we were printing it on the 3D printer. If I recall correctly I think we made the faces concave for style and then extruded up the numbers.
I have no need to do this, but was intrigued by the idea for a mathematical approach.
I little further into it; I have used equations to drive a part file that will generate all five of the platonic solids to a solid. The user inputs are the Id and type of solid wanted – i.e. size and number of sides.
The most pointless is the cube! The most difficult to fit in to my methodology was the octahedron. Was worth the effort to learn equations a little deeper, and use the newer style equation editor.
http://grabcad.com/library/platonic-solids-x5
I will stop now!