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Modelling an Archimedes' Screw

Monday December 9, 2019 at 4:25pm
Archimedean screws are often referred to as “water screws” since they are commonly used to transport water between different heights. We often see some of our customers do screw feeders and we thought it may be beneficial to create a blog documenting an effective modelling workflow to create your very own Archimedean screw. 

There are numerous types of screw feeders. In this blog we will review how to model a screw feeder that revolves inside a tube along with the water screw type.

Screw Feeder – Revolving Inside a Tube

Firstly, we will look at the type that has to go into a tube – one way to model it is to start with a big cylinder and cut away a big spiral groove.

So here’s my first feature, a 200mm x 1000mm long cylinder.

Then we need a path sketch and a profile sketch: -

Notice the path has been extended the length of the pipe – if we didn’t do this the swept cut would not break through at the ends.

Here is the profile sketch – in this case it’s been sketched it on the same plane as the path, which is not normally the plan for a sweep feature, but is preferred for generating our desired geometry in this instance.

The Cut-Sweep feature can then be used to remove the unwanted material: -

The trick is to use the setting “Specify Twist Value” over on the left where it says “Profile Twist.” Hit the green tick, and this is what you get: -

I did a little extrusion on either end, just to show where it would fit into the bearings.

This type of screw feeder would need to go into a tube: -

Generally, the tube is held stationary and the screw turns inside it, lifting liquids or grain or similar substances up the tube.   

Archimedes Screw 

Of course, I could have started with a small central cylinder, and used a Swept Boss to add the material of the screw’s “vane” – so then I thought, hmm, what if people need to do this on a regular basis?

Since SOLIDWORKS 2016 there has been a Thread tool – that can be set up to do what we want:-

What that command will need is a sketched profile, saved as a Library Feature into the location on your PC that is listed under System Options, File Locations, Thread Profiles: -

As standard that is C:\ProgramData\SOLIDWORKS\SOLIDWORKS(year)\Thread Profiles.

So this is the sketch I created in a new part: -

Notice the single 200mm vertical construction line going up from the origin?

If you have a line like that in your profile sketch, the Thread command will default to use that as the pitch for your screw.

Then you have to exit the sketch, but have the sketch selected on the tree, and then go to File, Save As and (before you browse anywhere) change your file type to Lib Feat Part (Library feature).

Then browse to the Thread Profiles folder and hit Save.

Then I started the part that was going to be my V2 screw with a long thin central shaft, and hit the Thread button: -

You need to pick a circular edge to tell it what you want to thread, and in the “Type” drop-down I selected my “Archi Screw” library feature - you’ll see that there are options to rotate or flip the profile if it’s not in the correct orientation.

The diameter of 20mm is defined by the circular edge I selected up the top. The pitch, (shown with the little red arrow) is defined by that vertical construction line in the library feature sketch.

You can over-ride this by pressing the button on the left and type in a different pitch if you need to.  If you are adding material you need to have the “Extrude thread” option selected shown at the bottom.

Hit the green tick and this is the sort of thing you can get: -

Ok, so far, so good.

But both of these would need to go into a tube, and both would leak due to the clearance between the screw and the tube.

Well, there is a variation that has side walls attached to the screw that rotate with it, sometimes called a water screw.

This could be created by a Swept Boss, but manufacturing that in real life could be a bit of a nightmare, so I thought that Sheet Metal would be the way to go.

This time I started with a short cylinder, as I only wanted to do one revolution of the screw to start with.

Then I drew a path sketch as before – the same length as the cylinder this time, and another sketch for a profile – this time as a single line with one end stuck onto the outside of the cylinder.

It is important that this profile line is spaced away from the path sketch – as we shall see next.

I then used a Swept Surface – with the option “Specify Twist Value” and just one turn: -

The reason for creating this surface is solely to use to create two spiral lines – each one in it’s own 3D sketch. So it is a case of opening up a new empty 3d sketch and using Convert Entities to put lines in 3d over each edge of the swept surface: -

Once that is done for the other edge in a separate 3d sketch, we can hide the surface body and see what we have: -

Then we can use the Sheet Metal command Lofted Bend and pick the 3d sketch lines: -

This gives a sheet metal body that will flatten: -

So, what about the side walls? Well, a circular sketch down at one end – with a small gap in it.

And then make a Base Flange feature: -

You need to decide how high up you wall are going to be when you do this – I went for 100mm, so I made the base flange tube extend 100mm past the top of the screw vane.

Then the cunning part – Unfold (not Flatten!) that body: -

Then we can cut away anything that we don’t want: -

And then use the “Fold” command to roll it up again: -

A Linear pattern to create as many bodies as are needed, and we’re there: -

This would go in an assembly something like this: -

To see the finished thing in action, watch the animation below.

By Rory Niles.

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