Hello, I'd like to give an update on my progress. Here is something that I tried over the weekend. - Created another mesh, using the PIV resolution. The refinement is done near the walls, atmosphere, and at the interface between the main channel and floodplain. - Ran a two-stage simulation: 0-40s using kOmegaSST, 40-80s using LES. To answer your question, my understanding is LES shows the instantaneous velocities, and I can see the progress of secondary currents over time. But please correct me if I am wrong. With the both turbulence models, the velocity magnitude on the floodplain surface is lower than that of the main channel, which is expected. With LES turbulence model, I can see secondary currents/upward movements near the interfaces at several x values (see images). However, they look smaller than what is shown in the paper. Is there anything which I can tweak? I also received some feedback from my peers, that I need to make the mesh more refined. It seems academic papers use much more detailed meshes (mm size) for LES. I am checking and considering this route too, although I am worried with the execution time. Thank you again for your replies! https://cdn.discordapp.com/attachments/400697259819270145/1557013916171763843/meshing.png?backend=b2&ex=6ac641b5&is=6ac4f035&hm=f0dc65eb98263a9ccce90a17178ca4916658f908936b884e629069c5d1a2ac2c& https://cdn.discordapp.com/attachments/400697259819270145/1557013917060833300/U.png?backend=b2&ex=6ac641b5&is=6ac4f035&hm=81a560c7c5c2e56c8b90b80a55ee15cf4940f2a0f5ae2015d4406cd831d347b7& https://cdn.discordapp.com/attachments/400697259819270145/1557013918159872010/secondary_currents.png?backend=b2&ex=6ac641b6&is=6ac4f036&hm=b4475773b3fac498a8fcc5b205efa2ee9378bc436ba58ff7105aa999fd0b2979& https://cdn.discordapp.com/attachments/400697259819270145/1557013919246319616/secondary_currents_paper.png?backend=b2&ex=6ac641b6&is=6ac4f036&hm=bd6ad04b67d5ce41b5e142829247e22ae2c60e1a9a1e405f5527a30ff79682e8&

(Btw, what is the proper etiquette for discussion here? Should I reply the older post or create a thread?)

That is super coarse, especially for an LES to be having physical meaning. But ofcourse, this is a very subjective and loose comment on my side. 1. As a starting point, stick to kOmegaSST for now, and consider your PIV level mesh as the coarsest resolution, now do ~1.4-2x in each direction and run again...check the difference in results. Repeat it for a third time... See if your results stop changing with mesh resolution. 2. Does the timeAverage of the LES field correspond well to the RANS field? 3. See if you can quantify the "smaller than what is shown in paper". (I am holding back on comments about behaviour near the free surface: the flat free slip condition may not be most accurate representation BUT it is too early to comment as you need to establish grid sensitivity first before we have confidence in your values) 4. The LES result is not instantaneous, strictly speaking, but yes it is supposed to represent the major chunk of instantaneous motion.. as compared to unsteady RANS which has an inherently averaged nature as conpared to the instantaneous manifestations of the flow..(to simplify: these differences are embedded in the formulae used to close the navier stokes equations using the assumptions of these models) Technically, they are both representative of only a part of the full velocity field, but ideally, a well-done LES would approach the true instantaneous velocity - so it does inherently carry a stronger instantaneous character and something you can consider as a reasonable representation of large scale instantaneous flow (I hope I don't killed by big dogs lopezcastano and zino on this one XD ). So umm do average things for LES when looking against PIV... For starters just simply use temporal Average over many steps in paraview.. I am curious how many cells are there in your domain?

Thank you, that's very helpful. The current cell count is about 900k cells right now, and yes that's very coarse. I will run the same simulation setup (RANS -> LES) but with finer meshes progressively now. Then compare the averaged LES results with RANS'. I wonder if the current duration (40s RANS - 40s LES) is OK though, or maybe I should run longer. As far as I know, the paper doesn't state much of the data. It only says something like: "On the other hand, case 2 and 4 both show oppo-site secondary flow pattern in large vertical scale (clockwise direction) on the interface between low channel and floodplain (z/B = 0.5) while anti-clockwise secondary flow around z/B = 0.4 is comparatively small." But I will see if I can derive something although rough from the images.

Btw, for averaging, I use OpenFOAM function like this. I wonder if this is correct.

fieldAverage1
    {
        type            fieldAverage;
        libs            ("libfieldFunctionObjects.so");

        writeControl    writeTime;

        window          20; 
        windowName      w20;

        fields
        (
            U
            {
                mean        on;
                prime2Mean  on;
                base        time;
            }
        );
    }

´window 20;´ gives you a moving average over the last 20 seconds, is that what you want ? However I am not sure with the syntax whether its active when it is not defined withing the brackets for e.g. the U-field ( so together with prime2Mean etc) Otherwise I think this should be good if you want to include every time step in the averaging.

Thank you. I don't exactly know what is a good value here. I think I will write several functions with different windows

But are you sure you want a moving average, and not just a regular average? In most cases you would simply use a regular average, unless you have a specific reason to do otherwise.

Rolling average is good to discard startup transience

but tbh I never really trust it and I just have the function object kick in from a certain time onwards

That is a good point! - but I usually also prefer to let the FO start after a settling period.

The rolling average algo is kinda suspect from memory

it doesn't do a real rolling average, because to do that you have to store the field at every point in the window (so you can remove data from the average as it leaves the window)

So you have a sort of setup where the contribution to the mean decays exponentially, but the values from before the current window are never truly gone

Does that mean OpenFOAM's rolling average is not accurate? Maybe I should use the temporal average in Paraview afterall 🤔

I think it's accurate if you use the EXACT mode

the approximate mode will be more of a filtered average

But exact mode requires storing the field for all the time steps in your window

which could be very expensive for storage space

I am not surprised the paper is not detailed - it is just a conference paper, you should look for something from the authors which got peer-reviewed.

For 40 s + 40 s ... monitor quantities at strategic points... using the probe function object... observe fluctuations at various locations and note whether they have entered an oscilatting/chaotic but stable behaviour. ie remain within some bounds... this will also tell you about period of averaging to get a clean mean flow structure, which is what seems to be plotted in the PIV images as well - it doesnt look like those are short term averages but the dominant rolls of motion, possibly determined from a large number of instantaneous samples. Finding a journal article by this group will help you get more detailed information - may not be the same authors but same laboratory, same supervisor, something like that.... if they have a piv and a test channell, it is likely that they published more than once using this setup.. I would suggest establishing grid sensitivity and statistical steadiness using your RANS result, before bothering with LES for every single simulation you run. @User

does anybody have any advice for meshing in CfdOf for freecad? i'm completely new and my meshing either takes forever or crashes, and idk if it's cuz i messed up the install or if it's cuz i'm just horrible at CFD. the few times i do get a mesh and run the solver it often just ends up crashing a few hours later too. any advice or just guidelines would be super helpfull :D

Very little info. What version of FreeCAD? CfdOF? Are you using gmsh or cfmesh? What is your goal? Are you on a capable computer and expect better performance? Keep in mind that installing gmsh or cfmesh with docker is not advised, as the docker image is outdated (I've been told so on the CfdOF forum, haven't confirmed it). It's best to install both manually and point FreeCAD to the appropriate install locations (I'm assuming you are on linux, I do not know what that process is like on windows). As for taking a long time: quadruple check all of your settings. You may accidentally be using way too fine of a mesh, or perhaps the algorithms for your mesher are simply not able to handle your geometry in a timely manner. There is no one single approach to meshing, it all depends on your geometry. If it's simple, then most people start with a coarse mesh which is then manually refined either via faces, edges or volumes (at least in cfmesh and gmsh workflows I've seen and used within CfdOF). For more complex geometries or setups, it may be beneficial to start with submeshes for individual faces or volumes and then join them together. From my experience, CfdOF is great for simple stuff while learning (since it's so seamless within FreeCAD), but it's extremely limited. I also believe it may even be detrimental when it comes to learning OpenFOAM, as you're not working directly with the files and not all settings are accessible from the GUI, so you're missing quite a bit of crucial information, which is important for assessing your result.

Ah, sorry for not having that much info, i’m completely new to CFD stuff so idrk what’s customary to include when asking for help so i just went for my general problem. I'm using FreeCAD 1.1.3, CfdOF 1.37.3, BlueCFD 2024, and what i assume to be the latest version of cfmesh (i couldn't find the exact version). My current pc setup has a ryzen 7 7800x3d, 32GB 5200MT/s ddr5, 2TB kingston NV3 nvme all on a b650e wifi. i also have a 3080, although i don't know how relevant that is since i don't think OpenFOAM uses GPU acceleration. I recently switched from docker to running stuff on my pc in hopes it'd run faster. I'm currently just trying to learn CFD basics, such as how the different boundries work and stuff. But most of the time either the meshing or solving ends up failing. For example i've tried to play around with the "rotating" boundry on this compressor i made, but sometimes the meshing takes upwards of an hour depending on if i put a casing around it and how big my medium is. I go with a base element size of 0.5mm which i don't think is too outrageous seeing as the model is only 100mm in diameter and the thinnest parts are 1mm thick. The few times i have gotten past the meshing and solving the data also seems corrupted somehow, i could just be interpretting it wrong, but it's all jagged and has colors that aren't on the scale. i'll try to find pictures later if i saved any. Thx in advance and let meknow if you need anymore info, as i said i'm very new:) https://cdn.discordapp.com/attachments/400697259819270145/1557636166046580796/image.png?ex=6ac88539&is=6ac733b9&hm=da8dd32adc900093e1886865a60d318ee5f0d3bf01cfcbd4db688e22912c6831&

Thanks for all the info. CfdOF has a dependency checker which should look something like this (it should be found under preferences for CfdOF): > Checking dependencies... > FreeCAD version: 1.1 > System: Linux > Runtime: Posix > OpenFOAM directory: /opt/openfoam13 > OpenFOAM version: 13 > cfMesh-CfdOF version: 1.32 > HiSA not found > Paraview executable: /usr/bin/paraview > Paraview version: 5.11.2 > gmsh executable: /tmp/.mount_FreeCAdJaiDo/usr/bin/gmsh > gmsh version: 4.15.0 > Completed CFD dependency check Your specs are very good, it should not take more than a few min to generate a mesh (of course heavily depends on the algorithms you use and how complex the mesh is). Sometimes the algorithm can end up in a loop trying to iteratively improve a mesh which ends up taking forever and still producing a very poor mesh. What exactly causes this is very difficult to pinpoint. A little explanation on CfdOF: it's doing nothing more than linking GUI buttons to regular OF commands. So when you press check mesh, it runs the checkMesh command and checks to see if there are any major issues. It will report as the mesh being ok in its own console, but that can be misleading. You should manually open up a terminal in the case and run checkMesh yourself, that should provide you with way more information. Then open the case in paraview and visually inspect the mesh (I recommend using the clipping tool with crinkling enabled, that way you can what the cells look like in 3D). Another possible source of error could be the geometry. I notice on your image that there are some edges on the fins, did you ensure you don't have any internal faces?

As for the settings for meshing, the base element size is just that, the base on which your algorithm of choice iteratively builds the mesh. What is more important is the minimum and maximum cell size. In my experience, both gmsh and cfmesh tend to use the maximum cell size wherever possible and smaller only if their algorithms determine the curve requires smaller cells. This tends to be quite unreliable, especially for more complicated geometries (in my experience).

I forgot to mention, but i’m running the latest version of windows 10, that might’ve been obvious from me running BlueCFD though. When you say esges which ones do you mean? I haven’t really had any problems with internal faces as far as i know, for example, it and similar models sliced and 3D printed just fine. Also, where do you set your maximum and minimum cell size? My GUI when meshing only has an input for base cell size. I’m not home right now so i can’t send a screenshot, but i’ll try to remember :>

> CFD basics > Compressors I joke but its not a trivial simulation. 0.5 mm max cell size is in fact quite refined for a 100 mm rotor. Compressors are rarely modeled in full, but a single passage only with periodic boundaries and mixing plane with the diffuser/volute. If the goal is really to just start CFD, you can start with a nozzle or diffuser if you want to stay if the compressor world to build confidence and a feel for that before going into that

I figured it’s a bit more complex for ”just starting out”, but it’s what i need to do for my school project 😅 If you have any good tutorials to simulate compressors or just progress with OpenFOAM as a beginner i’d appreciate alot if you could link them! I’ve also been thinking about moving away from CfdOf after finding out it’s pretty limited, it just seemed apealing initially to have it integrated into FreeCAD, but after doing a bit more research i think i’d be better off if i just made the effort to learn OpenFOAM. I’m very open to suggestions and help tho seeing as you guys seem to know where to start and stuff :>