Find Simulation answers, share expertise, and connect with your peers
Find Simulation answers, share expertise, and connect with your peers
For my master study internship project I'm trying to match experimental data (mainly drag values) for a free surface analysis of a surfboard. Unfortunately, the drag forces often differ easily 20-60% and do not show the expected results of increased drag for higher velocities. Is there anyone that could suggest improvements of my model, or show me mistakes I've made?
I thought this to be an interesting example case for free surface hydrodynamic simulations to share with the Autodesk CFD community. I'll explain the experiments and the model shortly. I've also added a screencast in which it is easy to see what setup and settings I used.
In the experiments, the surfboard is towed in a straight line in a towing tank at four different velocities. The board orientation (and therefore submergence) is fixed. Drag values and wake patterns are recorded. For the case showed in the screencast, the velocity is 4.55m/s and the experimental drag force is 104N.
The board is suppressed and modelled in a domain with an air and water box. Symmetry is not used for future research reasons. Inlet and outlet velocity can be set and the height of fluid initial condition is applied to the water volume. In contrast to the experiments, the water is now moving relative to the fixed board.
Manual meshing is applied. The refinement region nearby the board has an element size of 0.0125m. The board's surface is also meshed with this size. 10 wall layers are used, with a layer factor of 0.6 and gradation of 1.25. Wall layer blending is enabled. The Minimum Refinement Length was set to a minimum before generating the mesh of 3 million fluid elements.
A transient free surface analysis is performed with the SST k-omega SAS turbulence model and the ADV5 advection scheme. Generally, a time step size of 0.005s is used with 10 inner iterations. Intelligent solution control is enabled, automatic convergence assessment is disabled. Convergence graphs do not seem to improve anymore after 15000 iterations. Drag values are measured as the total x-component of the wall results on all the faces of the board. For the case showed in the screencast, a drag force of 42N is found, with a standard deviation over 5 measurements (each separated 0.2s) of less than 1N. Furthermore, I expect water to flow of the deck (top) of the board, but it doesn't, i.e. water with 0 velocity remains there.
I've got a few hypotheses why results are different between the experiment and simulation:
- The mesh is not mesh independent. I started a mesh independence study, but results on this fine mesh still differ quite a lot compared to the coarser meshes. Trying finer meshes is not doable with my resources, since I'm running in the cloud and simulations then have to be restarted every 3 days, many times.
- The mesh is not good. There might be ways to improve the mesh, without increasing the number of elements. Any suggestions?
- The y+ values are too high. I've found y+ values are reaching a max of almost 79, while less than 1 is recommended for SST k-omega (SAS). Can I decrease y+ by using a finer mesh?
- Surface roughness must be applied. When the board is suppressed, it has no surface roughness and the fluid might therefore experience less resistance (true?). I did a little test on this, added some surface roughness (0.1mm, 0.01mm and 0.0015mm) in the material (polystyrene) and did not suppress the board. Drag force of 44N was obtained (for all three roughness cases), so not much of a change. y+ values were slightly higher. Can adding surface roughness help getting drag values closer to the experiments?
- Something else is wrong.
Before concluding that the mesh is not mesh independent and that I simply need a better solver computer to solve for finer meshes, I'd first like to resolve all other potential problems.
If there is anyone that could help me with this case, that would be fantastic!
Thanks a lot in advance,
I just found out that Intelligent Wall Formulation was still enabled for my roughness simulations, while it should be disabled when surface roughness is applied. I hope to let you know the new results with surface roughness soon.
Thanks a lot for the clear and thorough explanation! This looks really interesting and I would be very happy to take a look.
Your setup sounds good and it does sound like a meshing issue.
Could you please upload a .cfz file here and I will see if I can get closer to the experimental data.
All the best,
Fantastic that you would like to take a look! :) I've uploaded a .cfz file here. The mesh and final results are not included, because the file was then too big to upload here... Just in case you want to see what the results were like, I added screenshots of the mesh setup.
Everything looks great with your setup! I think you could definitely achieve better results with effective meshing.
The issue is the triangular surfaces making up the surfboard CAD geometry make it very hard to have a mesh with smooth transitions or any sort of uniformity which could significantly aid accuracy in results.
Is there any way that you could create a smooth surfboard geometry with fewer and more uniform surfaces?
Regarding Y+ values have you used an isovolume to identify where the high values are? as long as Y+ remain below 3 or 4 on the entire board then we can be generally satisfied.
All the best,
Wow, This project look really nice !!
i don't know all the context but why you don't add fins on your surf i'm sure they can have an increasing effect on the drag values.
Also, usually when you surf water has different caracteristic like air bubble in it , which can increase the drag effect.
Did you consider the drag produce by the leash ?
Where the data came from , the data that you use to compare your data ?
Nice to hear you are also excited about the project! This is the start of a bigger surfboard performance project.
As you mentioned, the simulated situation is still much simplified compared to real life surfing situations. We'd be very happy to include fins, air bubble effects, roll&yaw angles, wave shapes, motion studies (actually floating of the board) and maybe even leashes in the future.
The simulations are trying to mimic experiments conducted in a towing tank (AMC, Tasmania) in which no fins or leashes were attached and the board moves through motionless water.
Thanks for your enthusiastic input!
Thanks for taking a look! Great to hear you think the setup is okay :)
The CAD geometry was created from a .STL-file with 23000 triangular faces. This had to be converted to an .IGS-file to import it into Autodesk CFD. But with this many faces, I found Autodesk CFD to run very slowly. Therefore I had to reduce the number of faces (the board in the uploaded .cfz-file had 2000 faces).
It's also possible to start from a .STL-file with a higher resolution (159000 faces) or an .OBJ-file with a low (12000) or high (79000) number of quad faces. I've uploaded these files here*. Please note that the model might have to be scaled (0.1 or 0.01).
So far I've not been able to generate a quad faced importable file that runs smoothy. I'm gonna give it another try today. In case you or anyone knows a way to successfully make an importable quad faced model with lower resolution (or maybe a surface model??), please let me know! :D
Regarding the y+ values: I'm afraid they are higher than 3-4 on the board. With this view, you look through the board directly to the bottom surface. When 'Min' is lowered, the board's deck turns blue.
Do you think it is possible to simulate only the region nearby the board? I already half rejected the recommendations of having 5-10 lengths upstream and 10-20 lengths downstream, but only simulating the flow nearby the board could greatly decrease the number of elements and speed up analysis. I tried this, but couldn't verify yet if results were the same for having a larger domain.
I'll keep you posted :)
*I was only able to upload 3 files, so I didn't upload 'Square STL HighRes.stl'. Please ask me in case you want it.
Unfortunately, I failed. In case anyone has a suggestion, please let me know.
I've uploaded a closed .stl file now as well (where the tail is not open anymore) and a .step of the body.
Is there a way to obtain two external volumes when doing a Surface Wrap?
I was able to do a surface wrap around the obj-geometry, but could only generate one external volume. Therefore I was unable to apply the proper boundary and initial conditions (such as height of fluid), because I didn't have a water and an air box.
I tried to export the CAD geometry from Autodesk CFD, so that the wrapped board could be obtained and two boxes could be added in Fusion360 or SimStudio, but exporting the CAD model didn't work (got an error).
I was also thinking about using the surface wrapper but sadly I don't think there is a way to apply two external volumes.
I think you should stick with the larger domain as if the slip BCs are too close to the model flow vectors may point into them causing a crash.
I think once the CAD has been cleaned up we should be able to get appropriate Y+ values. Ideally we need the geometry to be only a few surfaces.
In your CAD software is there some way to merge surfaces or create an envelope around the board? I am not very experienced with CAD so I will ask around. Which CAD software are you using?
We are not the most experienced CAD folks here, by definition. Where'd this CAD originate from? Fusion 360? Inventor? I had a colleague of mine take a quick look at it and I think there is a way to smooth these surfaces out to make a continuous body (for lack of a better description).
Maybe you can post of the respective CAD forum and try to get some help there? Those forums are usually packed with knowledgeable folks.
Thank you for your answers :)
I think it is indeed a good idea to post the CAD related question on another forum. I'm using Fusion 360 and have been trying things with FreeCad and Meshlab for this project also, but SolidWorks or Inventor would probably have more features and I can use them also.
Do you know if Autodesk CFD also accepts curved edges and faces, instead of being build up out of many straight lines? That should be great.
I shall give the simulations a try with a surfboard consisting of less surfaces. I'll see if I can get the y+ lower. But unfortunately the entire study is about the surfboard performance due to the board's geometry, so the shape should be well represented...
When I won't have any interesting updates soon, I'll accept one of your posts as the solution. In case you hear a possible solution from one of your colleagues, please let me know :) Thanks a lot!
CFD Is perfectly happy with curved surfaces and edges! There is no need to make the board out of small straight edges, in fact this is where the meshing problems are being introduced.
Good luck with the modelling and let us know about your progress as its a very interesting free surface application!
All the best,