Review of OpenFOAM: free CFD

[cfd_guy]

Originally Posted by julien.decharentenay

I was wondering if there was a single document covering issues such as:

- geometry: What simplifications are "acceptable"?
- size of the computational domain, incl blockage ratio, number of length before and after;
- mesh such as first layer size, number of layer in boundary layer, mesh resolution in near and far field;
- boundary conditions;
- physical, incl turbulence models, and numerical models;
- typical validation models;
- and ideally a discussion on limitations.

If you have access to the Ercoftac BPG, I would be looking for something similar but applied to the automotive industry.

1. geometry: What simplifications are "acceptable"?
This is a tough one to answer because it just depends. It depends what the end goal of the project is and what kind of accuracy you are looking for. Example: You could have a much more simplified model if you are testing basic front end designs, than say if you are testing underbody flow for engine cooling.
***My usual simplifications: simplified underbody (not just flat however), simplified suspension and brakes, simplified engine (if I even have an engine(ony when using porous flow through a radiator)), and I am sure I am forgetting a few others.

2. size of the computational domain, incl blockage ratio, number of length before and after
The size I usually use is 5x length in front of car, 15-25x length behind, and 2-5x length on sides depending on the project. I do not know if this is industry standard or not, just what I picked up from one of my professors. I never thought of calculating blockage ratio however since I have only used that when looking at a windtunnel. Computational domain depends really and everybody will give you something different. I think you need at least 5 million for normal automotive, but more like 25 million for a complicated open wheel car.

3. mesh such as first layer size, number of layer in boundary layer, mesh resolution in near and far field
I use yplus for this. I just keep a yplus that is acceptable for the turbalance model I am using.

4. boundary conditions
The normal for this I guess. I do rotating wall velocity for the wheels. The walls are set to the internal velocity field so wall velocity to not see boundary layer growth.

5. physical, incl turbulence models, and numerical models
For turbulance models, I usually use k-omega SST because I like how it correlates pretty well but takes longer to converge than say a k-epsilon. I would say that the three most common for steady state analysis is k-epsilon, k-omega, and k-omega sst. LES and DES are becomming more popular however with computing power increased. I will occasionally do a transient analysis, but most cases I can get away with steady state. I normally use a steady state incompressible solver except if I need transient or compressible (dragster).

6. typical validation models
The ahmed model is the most common and what I have used. I have also been able to validate a case using a windtunnel also.

7. and ideally a discussion on limitations
Really just depends on the knowlege of the engineer, time, and computing power. Plus a little common sense

I hope that is clear. I could go further on some things but that is the jist. Plus I have a case to setup

[julien.decharentenay]

Thanks a lot for the info. I seem to understand that your best practice are derived from experience, rather than taken from literature - although most looks pretty much common sense. Is this correct?

A quick question on the Ahmed body. My understanding is that the measurements are focused on the pressure in the rear body (particularly on flow field vs rear angle and flow detachment). How are you fining correlation between k-omega SST and experiment? I was under the impression that the "standard" was linear k-epsilon with non-equilibrium wall function. What is your experience?

[cfd_guy]

Originally Posted by julien.decharentenay

Thanks a lot for the info. I seem to understand that your best practice are derived from experience, rather than taken from literature - although most looks pretty much common sense. Is this correct?

A quick question on the Ahmed body. My understanding is that the measurements are focused on the pressure in the rear body (particularly on flow field vs rear angle and flow detachment). How are you fining correlation between k-omega SST and experiment? I was under the impression that the "standard" was linear k-epsilon with non-equilibrium wall function. What is your experience?

More or less yes. But some of the info from working with my professor was from literature also. I used a both approaches as there is no set in stone best way to set up since all cases are different.

Yes the Ahmed body is to study the separation of flow on the "hatch"/slant of the bluff body. It is also good way to study the wake. You are correct in saying that the the k-epsilon is considered standard and it also correlates better to the windtunnel data from the ahmed study. In most cases I ran with different turbulance models, k-epsilon showed a slightly higher drag and lift value. This correlated closer to the actual measured drag and lift.

After that, you might be wondering then why I don't use k-epsilon. The reason is from talking to more experience people than myself about its correlation to real world motorsports cases. I discussed this in detail with one. Basically they noticed that the k-omega sst model worked better in cases with high separation. Since most actual cars and racecars have a good amount of separation of flow, it usually is gets better results. ***Other people will disagree however since I know many who still use k-epsilon*** Also remember, it is just a mathematical model to represent the chaos that is turbulence.

[julien.decharentenay]

Thanks again. If you don't mind me asking:

- Are the pictures you posted earlier generated with EnSight? They did not look like the typical ParaView pictures associated with openFoam simulations;

- What hardware and simulation turn-around time do you use of a typical simulation? Is it in-house hardware?

Thanks.

[cfd_guy]

Originally Posted by julien.decharentenay

Thanks again. If you don't mind me asking:

- Are the pictures you posted earlier generated with EnSight? They did not look like the typical ParaView pictures associated with openFoam simulations;

- What hardware and simulation turn-around time do you use of a typical simulation? Is it in-house hardware?

Thanks.

Yes. I had access to EnSight for a while. I love it personally and I am looking at picking it up soon. It has more options and math available than ParaView. I am currently using ParaView however since I no longer have access to EnSight until we decide to purchase it

I use a small cluster of workstations obviously running linux. Depending on the size and convergence anywhere from 18-48 hours. It is in-house, but I did try amazons ec2.

It seems you have extensive knowledge of cfd and openfoam, what is your experience?

[julien.decharentenay]

You would need to clarify what do you mean by experience? Experience as in "what is your opinion of ..." or as in "how many years have you been doing...".

To keep to the thread, my experience with openFoam is quite positive (although limited to the last few years). I tend to limit myself to the existing solvers - I am not too much of a compiler of other people software (particularly when there is a lot of dependencies - although I am trying to compile ParaView at the moment). I am using openFoam on Windows (mainly) and ubuntu (on amazon ec2 and a local very old computer).

My application field was focused on HVAC applications up until last year, but has been focused on car aerodynamic recently.

My centre of interest is in the software development and coupling of tools together. Part of my recent projects includes:

- Khamsin, a SketchUp Plugin for CFD Modelling - which couples to openFoam as one of the CFD engine;
- Aerodynamic on Demand - a CFD based aerodynamic calculator for cars again based on openFoam and using amazon ec2;
- Khamsin Virtual Racecar Challenge - a virtual racing car challenge (for fun).

Feel free to check my profile on LinkedIn if you want a full detail of my experience.

[christofoo]

Originally Posted by cfd_guy

...
I hope that is clear. I could go further on some things but that is the jist. Plus I have a case to setup

Friendly nag.

Originally Posted by julien.decharentenay

...
- Khamsin, a SketchUp Plugin for CFD Modelling - which couples to openFoam as one of the CFD engine;
...

That looks interesting. Any thoughts on how useful Khamsin is? Any screenshots? A good tool like that could push me to learn Sketchup (vs Solidworks).

[julien.decharentenay]

Originally Posted by christofoo

That looks interesting. Any thoughts on how useful Khamsin is?

I am not the best person to advise on how "useful" Khamsin is. You can have a look at the work done by Andy Laurence Blog. He initially used Khamsin (looked for older post) and moved recently to Aerodynamic on Demand. These are two different front ends to more/less the same CFD engine/

The overwhelming feedback is that it takes a few hours and a bit of frustration to get the setup right with Khamsin - my apologies. See CFD With Sketchup - YouTube for example.

Both of the above are unaffiliated.

Originally Posted by christofoo

Any screenshots? A good tool like that could push me to learn Sketchup (vs Solidworks).

If you have a bit of time, I would recommend watching one of the analysis video. A good one is: CFD Modelling of a 250cc kart - YouTube or any other from the YouTube channel http://www.youtube.com/user/HibouSoftware. Otherwise let me know and I can send you a pdf of the documentation/tutorial.

Sketchup vs Solidworks: I will doing a web presentation on some of the limitations of SketchUp for CFD applications that I have identified while using it in the future. A main one is its inability of properly handling curves... Best way to keep informed would be through twitter @HibouSoftware or Google+ (info@hibouscientificsoftware.com.au).