Modelling a propeller
I'm currently attempting to model the flow through and around a propeller designed for a remote control aircraft. It'd be much appreciated if I would be able to get some feedback on the method I've used as I'm a complete novice when it comes to CFD.
Firstly, I modelled the propeller shape in catia, saving it as a .stp file, before importing it into cfd. I then created a cylinder surface around the propeller, sizing it just so it covered the propeller, then created a larger block surface that housed both propeller and cylinder (this block surface acting as the wind tunnel).
Next I created 2 regions out of the cylinder surface and the rectangular surface, before subtracting the propeller out from the cylinder. This left me with two regions (the block surface, and the cylindrical surface minus the propeller). I split both the block and cylinder into different faces.
I then created two meshes in the continua folder, so it'd be possible to assign a different mesh to each region. I then applied the mesh.
Next, I used the tools section, and the motion node, I selected to choose a new rotational motion, assigning the axis both direction and an origin, choosing a rotational speed (whilst leaving the "managed coordinate systems" and "coordinate system" settings as default.
I then went back to the regions folder, selecting the region with the cylinder surface and propeller, then assigning the rotation I'd just created as the regions "motion specification".
I then specified the physics model, at first I tried creating 2 physics models so as to assign each region a separate one. This encountered an error, so I settled for a single physics model (choosing Implicitly Unsteady, gas, coupled flow, ideal gas, turbulent flow, k-epsilon turbulence). I then set the initial conditions; pressure 101kpa, and I set the velocity to 10m/s.
I then moved back to the regions folder, changing the front block face type to "velocity inlet" whilst changing the rear face to "pressure outlet". In the region containing the cylinder surrounding the propeller I changed the front face to "free stream" to allow the flow produced at the block inlet to flow though to the propeller. I also changed the rear cylinder face to "free stream" allowing the flow to pass through into the block.
I then set the stopping criteria to a suitable amount.
This is the process I've used so far, is this acceptable, or have I made some fundamental mistakes? I'm probably completely wrong. Also, any ideas on how best to display the forces produced by the airflow rear of the propeller. Any help/ constructive criticism would be greatly appreciated. Thanks.
A couple of things:
1) Unless you have computational resources, or a lot of time on your hands, then designing a propeller purely in 3D Navier-Stokes CFD is not practical.
2) For starters, check out some optimization codes like XROTOR, or the spreadsheet that someone put together in the link below:
3) After you have done that, or if you just want to visualize the flow, check out the Rotation System tutorial in Star-CCM+ help file.
4) After the above, you will realize that the faces of your cylinder should be set to the interface boundary type (accomplished by right-clicking copies of the cylinder face in each region and creating an in-place interface).
5) You should have also assigned (or split) the cylinder faces into a group that represents the propeller. With these faces, you can create force and moment reports in appropriate directions to obtain thrust and torque.
Thanks for the reply F-W, I wasn't actually trying to optimise the design of a propeller using CFD, in fact I ran a blade-element momentum theory matlab code optimising a propeller and the cfd analysis was just to compare results to see how similar they were.
I tried a few simple propeller type designs first to get the right method, and once I started using the more complex designs (the propellers created from Catia V5, by importing a number of aerofoil coordinates at different stations along the blade) Star didn't like it. The more complex models seemed to import in two parts, though i combined them before creating any block surfaces, and as I began the meshing procedure either one section would disappear, or both blades leaving only the hub. Is this due to the base size being too large?! If it is, unfortunately the computers here at university aren't powerful enough to cope with any smaller cell sizes than the ones i'm already using. So if that's the reason, this may be a lost cause.
The tutorials on meshing and rotating systems in the help system is my best advice, without me having to iterate pages of the same material. I also suggest seeking the university's resident Star-CCM+ expert. If the project is big enough, cd-adapco might provide some consulting and assistance as well.
In the meantime, tell me the specs of the PC, and I will let you know if it's even worth the effort.
In general, it's okay, but
1. I would have created the cylinder at a certain distance to the propeller tips. You should never put the interface to a point where the flow changes much. Just consider vortices, pressure gradients, velocity gradients etc. The more far away it is, the better it is.
2. Additionally to F-W's hints, you also should also create an interface from the perimeter of the cylinder. F-W wrote it correctly, but it's easy to overlook that.
3. Is the flow really a compressible one? I think, it will be not necessary to use an ideal gas model at a flow velocity around 10m/s. Keep it as simple as possible.
4. (just a minor one) It is not necessary to create two mesh continuas. One single mesh continuum can do it as well.
5. Create some reports for the forces. The force you are interestet in doesn't act on the flow behind the propeller, it acts on the propeller surface itself. With that report, you can create monitors and plots, so you can display the forces over time.
|All times are GMT -4. The time now is 21:01.|