As always, the AMA was interactive, and people are invited with follow up questions at any time of the zoom… ✨✨✨
The zoom lasted two hours (more than twice longer then as planned!!) many more questions were answered, besides those raised upfront.
The recording is processed (due to me being a technical dummy… 🙃, and thanks ‘to my dear friend Rajat Walia) has finally been added as raw unabridged!
The links for the resources shown in the AMA appear in the post (other resources were handed on a private layer to certain participants and will not be shared here).
I am a Senior Lecturer teaching Thermo-fluids (not CFD) to Mechanical and Aero undergraduates at a UK university. My queries below are on behalf of some of my students after collating their queries. Hope you can spare a few minutes to help these future engineers (and also to help me so I can help any other students asking similar questions).
I did my PhD in the UK over 20 years ago and I have not used CFD since then. That means, I cannot remember some of the things I did during my CFD times. Still, some undergraduate students bring their CFD queries to me. I used to think I was OK with general CFD but after reading your posts on “all about CFD” blog, I have been very humbled. I rate my CFD knowledge now to be about xx% of your knowledge. Therefore, when students come to me with CFD queries, I give them your blog URL. They still come back to me with new queries when they could not understand something from your blog, which is not meant for the absolute beginner.
I have listed a few queries below. PLEASE see if you could offer us some answers. (You could even use the answers you give here to further enhance your existing blogs).
Your blog post https://cfdisrael.blog/2019/10/10/turbulence-modeling-best-practice-guidelines-standard-evms-part-ii/ says “…it is incorrect to refine a high Reynolds wall-sensitive model such as the standard k-ε such that the first grid away from the wall penetrates to the viscous sublayer“. We should try to have the first cell centre y+>30 away when wall functions are used. k-epsilon needs this first cell centre outside the viscous sublayer but k-omega needs an inflation layer (about 15 cells as you recommend) in the viscous layer even if k-omega uses wall function. How would someone decide whether the first cell centre should be outside the viscous sublayer ? Simply put, how would a user determine if a turbulence model is wall sensitive or insensitive ?
When I repeat Florian Menter’s general rule of thumb of 15 orthogonal to the main gradient of velocity (i.e dU/dy in a conventional sense) I refer to the entire boundary layer, and not to the viscous sublayer. The Standard Launder-Jones k-e model is a wall sensitive model, meaning it’s a high Reynolds number model, and the epsilon equation cannot be integrated through the viscous sublayer. So one either has the choice of placing the first cell away from the wall at y+>30 and using wall functions or if the flow is such that an important parameter such as drag should be calculated place the first grid away from the wall at y+<1 and use a low reynolds model for compensating the fact that model is wall sensitive (formally some highly nonlinear damping function such as Van-Driests – I wouldn’t like to refer to a specific way Fluent does that – but there there are the options of enhanced wall treatment or Menter-Lechner near wall modeling).
The COMPLETE boundary layer should have at least 15 layers NOT the viscous sublayer in case it needs to be modeled.
The k-w family is wall insensitive, meaning there is no wall treatment needed, that’s why in almost any case the SST version of k-w is preferred, here’s a pdf about the k-w evolution, very well comunicated:
Of course if one doesn’t use the right resolution to model the viscous sublayer, one would get erroneous results for cases of drag calculation for example.
Your blog post https://cfdisrael.blog/2019/10/05/turbulence-modeling-best-practice-guidelines-motivation-and-standard-evms-part-i-a/ says “The first cell away from the solid boundary (to be more precise, the center of the cell), should be located at y+<1 “ for resolving viscous sublayer. Should a user first calculate y+ (dimensionless) and then find the corresponding y (dimensional) in meters so the first cell height could be decided ?
Yes, the user should estimate a y+ by some means (he may also google for the Pointwise y+ calculator and just enter the estimated length/velocity/dynamicviscisity/dnsity and the y+ he is aiming for and he will get an estimated Re and a physical y for the y, he may use to mesh by some method available as first cell away from the wall, the iteratively check the y+ value locally through the simulation.
You should pay close attention that the log layer formally starts at y+=30 but its height in wall units depends upon the Reynolds number, meaning for low reynolds number applications such as ones on the verge of transition (some turbomachinary applications for example the log layer could be as thin as non existent though one still needs the right resolution to capture it. While in A/C applications the log layer could stretch for a few thousands and more.
You had indicated that in some cases, we need not 15 but even 40 orthogonal prism layers in the viscous sublayer. Could you give an example or two where such fine meshing in the viscous sublayer is needed ?
ANSWER: Usually in cases where the margin of security is taken to be as low as possible (due to weight/money) constraints for example) where very high post processing resolution is expected to find the calibration constants due the work every wher they would use even 40 inflation layers to cover the boundary layer. The aerospace industry is the best example for that.
You mention 15 or so cell layers in the viscous sublayer. Will the buffer layer be automatically dealt with by the models used ? Do we not have to worry about the cell sizes in 1 < y+ < 30 region?
Again, Florian Menter for example gives the rule of thumb for at least 15 layers in the ENTIRE BL. If one decides to use a wall sensitive model like the scalable wall functions than theFluent for example would scale any y* to be >11.225 as wall functions and every y*<11.225 as inside the viscous sublayer and use wall treatement. No buffer layer specific considerations should be taken. Fluent decides log layer or viscous sublayer accordionists to the y+<>11.225 automatically…
You have an image (file name “y-procedure”) with the heading “example in predicting near wall cell size” showing a calculation of y+ in your post https://cfdisrael.blog/2019/10/05/turbulence-modeling-best-practice-guidelines-motivation-and-standard-evms-part-i-a/. In that “slide”, there is a mention of a previous slide when it says “Recall from earlier slide, flow over a surface is turbulent …”. Do you think you can make the full set of those “slides” available at all ?
Actually I don’t. There is calibration part for a turbulence models, and it refers to a flat plate boundary layer without an adverse pressue gradient for example.
In the same post as in (5) above, you have a contour plot named “Eddy Viscosity Ratio contour plot” . There you call it a “good” boundary layer resolution. You state that “The best way to check whether the orthogonal layers cover the entirety of the turbulent boundary layer is to present contours of the Turbulent Viscosity Ratio“. Are those 15 orthogonal cell layers in the ENTIRE BOUNDARY LAYER or just in the VISCOUS SUBLAYER ? it has confused some of my students to think that the 15 cells should cover the entire turbulent boundary layer, even if I had suggested that the fine cells are only in the viscous sublayer and not even including the buffer layer. (These students believe you more than they listen to me : -)
The entire boundary layer and watch out that the maximal value of that ratio is somewhat in the middle of the boundary layer but should always be inside the BL, meaning covered with prism layers.
If the 15 layers cover the entire boundary layer then how many cells should be in the viscous sublayer ? Or should we simply ignore the viscous sublayer ? Also, should the 15 layers be in a distance corresponding to y+=30 ?
The 15 layers is a minimum resolution rule of thumb by Dr. Florian Menter. Remember there’s a growth rate which should be approximately 1.12 for the cautious ones and there are some methods to build an inflation layer which would give different built boundary layers (smooth transition, first height, last ratio, uniform)
Usually the prism cell layers (these 15 cells that you mention) roughly have the same height along the length of the surface and can be more like long rectangles. At the same time, we know that turbulent boundary layer height grows. If the 15 cells cover the boundary layer, then should those 15 cells also gradually grow in height as we move downstream, kind of causing the cells to look like
As a direct continuation of what I’ve wrote before, yes it will, it should also connect corners and meeting point (it does that by certain algorithms like stairsteping for example, meaning starting elliminating the number of layers like steps towards the corner, there are other methodologies to…) , the point of the matter is that we hope for the flow in most of the boundary layer the flow gradient is perpendicular toth prism face hence minimizing the calculation of derivatives error. It’s a wonder we can handle such complex geometries now. But rememe, this is only RANS, not LES, only first order simple flows which abide to the law of the wall which is a calibration over a flat plate BL gives good average first order results… lol
Do you suggest that getting y+ calculation wrong can be critical ? Students cannot find all the values need for y+ calculation for every application and they may have to estimate, “guess” estimate or use something oddly similar and this very likely give an incorrect y+ value, resulting in wrong size for the 15 layers and also where the first cell centre should be.
Just estimate ones than iterate and post procecess for y+ on the surface, then if there’s a large difference factor and remesh. You would see if you check that the length scale size doesnt have much impact on the y+ result (something like Fourth square root, so you may even leave the estimation as L=1 while estimating by hand or by the Pointwise y+ calculator)
One student wants to simulate liquid flow through a syringe needle and another one is trying to simulate the air flow through a very thin slit like a hand dryer. The hole diameter is so small in the syringe and the air slit height is a fraction of a millimetre. We are not sure about getting the boundary layer defined or deciding the number of cells in the inflation layer or the first cell size/location or the choice of the turbulent model. Any kind advice please?
Is the flow even turbulent in such tiny diameters of Poiseuille flows, if there’s an exit jet of course it is a turbulent jet due to the strong instability in the outlet but Im not sure, how to answer. If it is turbulent, simply have a lvery large aspect ratio and check for sensitivity in the number of bl cells, maybe 10 are enough for good enough resoluurion…
This is for my personal knowledge: You seem to have a deep theoretical knowledge about CFD fundamentals. In https://cfdisrael.blog/2019/10/05/turbulence-modeling-best-practice-guidelines-motivation-and-standard-evms-part-i-a/, you said that a poly-mesh with 12 faces have “has 6 optimal direction”. I did not understand this and do you happen to have a picture showing this or could you suggest some reading where I can read a bit more about this, please ?
Yes. Read my post about mesh quality, the one with the pretty yellow featured picture with the Polyhedral hive of 🐝 :
What is a good choice of turbulence model for simulating air flow in air-conditioning ducts, please ? There is a lot of turbulence at the vents when air is coming into a room. Also, the ducts can have roughness due to dust accumulation. Then, circular metal ducts are made by winding a metal sheet and therefore they come with a spiral seam causing turbulence. Then, further turbulence is added where there are fans or blowers in a duct. I have not able to guide our students on this. Similarly, simulating the liquid flow in a pipe after pump is also an issue as we assume no turbulence immediately after the pump when we know there is a lot of turbulence. As we do not know what to specify as the turbulence condition soon after the pump, we simply define a uniform velocity inlet boundary condition for the pipe, knowing it is not correct. I wonder if you have any suggestions, please.
You may use now a non uniform inlet condition without UDF, just with expressions. I can send tou an example if you like, usually if it’s swirling flow use k k-w sst with curvature correction.
And some none CFD questions because we are people networking not a data delivery mechanical system… 😊
You had written that you meditate for 2 hours from 4 am. Firstly, how many hours of sleep do you get each night on average ? secondly, what do you meditate on for such a long period ? I am a Buddhist and I am surprised in a “I want to be like that” kind of way as my meditation sessions are usually 10-15 minutes. You are amazing to be able to meditate that long.
Meditation is a fist person glance at our monkey mind. I enjoy practicing it and maybe somewhat addicted… 😉
I do it mainly to keep my attention and mindfulness of our only one and awe amazing world awareness and to be able to be a more compassionate person (a Bodhisattva striver… lol)
Your profile picture with a bold head gives the impression of a thin bloke but there is a photo of some well-built, mucho man with two kids in your “about me” page. Is that you in that heavy built guise as well ?
The picture with the kids is kinda old, they are already 11 and 7, and I’m not so muscular anymore…. 🤷🏻♂️
The one I used in blog was simply one I loved the best. Thats a picture I did for Tobias Holtzmann OpenFOAM site and it really came out nice in my eyes, like a lucky awesome photo for a very unphotogenic dude… 🤦
() Your parents were software engineers. You ended up in a similar area. Are you pushing your kids in a similar direction ? At least do they enjoy your CFD (I mean “Colourful Fluid Dynamics” as they see CFD) ?
No… I wish a Meta for my kids:
May you be happy, May be safe, May you leave with ease, May you achieve fulfilment… 🙏🏻
Unabridged Recordings and Resources from interactive AMA 2
(we’re sorry for some slight technical faults, they will all be corrected next AMAs)
PART I of AMA 2 (video unabriged recording session):
PART II of AMA 2 (video unabriged recording session):