CFD Analysis of MVG's
I have to do CFD analysis on MVG's on NACA 0015 wing and then I have to compare results with that of wing with no MVG. I have done the wing with no MVG.......but I am unable to capture the flow physics around MVG's .I have very limited computational resources ..I am using corei5 2.5 GHZ processor with 8 GB of RAM .around 3 million grid size is the upper limit.
What I have studied so far is that models that I can apply in this case are.
1) SA (y+= <3 ,30-300)
2) KW (y+~1)
other models like RSM and LES are just out of question because I can not resolve under y+1 with the present resources.
Currently I am working on a segment of wing with a pair of MVG's and I am using SA model. I am using ICEM for meshing and have made unstructured mesh around the geometry........and structured mesh in the rest of the domain.By that I can only achieve y+ around 100-200.With current configuration I am getting the flow separation even earlier than the simple wing case at 15 degree.Re 2.5 * 10^6
My question is
1)Is SA model capable of modeling MVG's.
2)Refinemet in ICEM to get y+1 with minimum possible grid size.I have tried to make a prism layer around the wing geometry but it gives worst quality due to the irregular geometry near MVG.So I am using tetrahedra to capture the boundary layer effects
3)What I can do with the present resources to capture the basic flow phyiscs around MVG....and what I can do in post processing to analyze flow physics around MVG and to see the vortex structures...
I need urgent help....I am only left with a month to present my Analysis.
I worked with SA and a structured grid to model a basic MVG on a flat plate with decent results.
Have you considered using a mesh free approach, where instead of fully describe the MVG you simply use a source term in the equations for it?
If flow details are not important you can save some cells and the flow becomes identical, say, 10 MVG heights downstream.
Google "micro vortex generator source term" for more info.
Thanks for answering :)
Uptil now I was only trying to model the MVG geometrically and then fine mesh it.
Yup I am now considering to model effects of MVG's rather modelling it geometrically. I have not done programming to make UDF's.Can you share with me the code you have used for the source term for MVG. After reading your answer I have started to study different models that are used to model the effects of MVG by adding source terms in NS equation. What I have studied so far I have known that it simulates the lift force generated by MVG. Certain parameters and the grid volume where the source term have to be applied is to be defined
Can u tell me what I have to learn in UDF to program the source terms and to apply them to specific grid area only ??
what grid size you used where u applied source term???
I am sharing the geometry image. I am using vane type MVG's.They have basically triangular shape so which model is better in my case.
It would be appreciated if u share a good read on UDF's related to my case.
it was really long time ago that i worked on this and i don't have anymore any of the related stuff (i mean, the actual UDF i used). This is not random, because at the time i was a beginner and it all seemed huge; now i see it more clearly for what it is, really standard stuff. Also, today Fluent is quite different and i would write the UDF quite differently.
If you can give me your email i can send some of the references i have on the source term in general. For the UDF you have to relate to the manual.
Generally speaking what you have to do is:
- write a define on demand UDF which will mark the zone where you want the source term. there are a lot of possible choices on this. At the end, we found that selecting the bounding box of the MVG as domain for the source term would finally give a model independent from the model constant for sufficiently high values of the constant. Another option is selecting just those cells being cut by the MVG, but then the model constant has to be somehow calibrated. The marking process itself is some cycle on the grid cells and when some conditions on the cell center/nodes coordinates are verified you say that, for example, a previously activated UDM is 1; otherwise it is 0. The UDM has to be activated before executing this routine.
- After this cycle is exacuted, before the calculation, you need to separete the marked cells from the rest. This involves first marking them (in the adapt part of the menu) trough the UDM you just defined and then separate the marked cell zone
- After this separation you can activate the source term just for this separated cell zone. The source term will then just be the replication of a given formula. I used the model of Bender, Anderson and Yagle. We found also important, for the convergence, the inclusion of the source term implicitly, which in Fluent requires the inclusion of the source term derivative with respect to the three velocity components.
- finally you can just run the simulation.
As inexperienced user (it was my first contact with Fluent and CFD in general) it took me 2-3 months to get it work. For an experienced user it is just a one day work (i can only imagine how frustrated was, at that time, my thesis supervisor).
For what concern the grid refinement, the basic idea of the model is that it should run without sufficient refinement, otherwise you could just insert it for real. I can suggest to work with a grid which is just sufficient for the rest of the flow without the MVG and calibrate the model constant consequently. Of course, the more you refine the grid the more the model will give you details as for the real MVG.
Finally, some works showed that for the specific model i used, MVG geometry details were unimportant. You will also notice from the model equation. This means that you only need few geometrical details of the MVG to be included in the model, like the area and the two linear dimensions.
sadly there are no conference proceedings from Ischia (i guess it is standard for the ERCOFTAC Drag reduction and flow control meetings).
I don't know how much i agree on this RANS-LES difference. I guess there might be a range of Re and MVG dimensions for which the boundary layer is correctly resolved but the details of the MVG are still unimportant (to some extent). However, if i had to bet money, i would agree with you.
Sinisa Krajnovic worked on this in LES, indeed without any model:
I really appreciate your help....my email address is firstname.lastname@example.org .I have also started working in fluent just a few months ago for my project so it will take sometime to learn the programming for UDF's. Due to shortage of time I have to stick with the previous approach otherwise the free mesh approach looks preferable. But in free time I would love to use that approach and compare the results.
Meanwhile I was just finding out the ways to mesh finer and finer and get near to y+ 1 with minimum grid size increase , finally I am successful doing that. The results that I got are good to predict the separation point and also shows delay in separation with MVG's attached,there is also a slight increase in lift coefficient but I am not able to comprehend one thing that pressure drag has increased with MVG's attached which is giving total drag coeffient to be higher.On the other hand I also havesuspicion on viscous drags. I am attaching some of the pics here so you can comment what I may have done wrong or can do better.
the flow is coming at 15 degrees of AOA at .12 M Re=3* 10^6.....There is circular Boundary having velocity inlet conditions and I have used default discretization schemes.
Can you help me figuring out how I can get somewhat reasonable values for CL and CD. I am using K w model with y+ about 2.5
from the velocity contours with the MVG i think it is possible that the case still has to converge as the low velocity blob behind the profile seems quite unnatural to me.
Also, consider that a lower drag with a MVG can be achieved only in certain conditions and not a priori. You will usually need an optimization process for this (and that's another reason why a source term model can help).
It seems that the main difference is in wing-le/lw ,which surfaces are these?
yup u r right it had not converged ....the CL and CD values were changing very very slowly for about 1000 iterations. the residuals were down to 10^-4 but as i gave it more time to simulate under lowered residual values the residuals started to jump again after some time......I think the quality of mesh is not quite enough ...I am using a non conformal mesh......unstructured mesh around 2 of the mvgs and structured mesh around the wing and rest of the domain.....to refine more I think I may have exceeded the node tolerance....but its quite frustrating to me because I have made no. of meshes with unsuccessful results...optimizing it again and again......decreasing the value of y+ adapting the mesh ...right now i m quite puzzled what to do next may be i shud start working on adding source terms the scary thing is if i start doing too many things i may end up doing nothing :(.......second thing I want to tell is that i am using K value to be .01 and omega value to be 1 ..the domain is basically circular extruded to make a cylinder.....I have used symmetry conditions at walls adjacent to wing and velocity inlet for the whole boundary.the boundary is 2c before the wing and 3.5c at wake......similarly about about 3.5c up and down..I think I should increase it.
the le is for leading edge and lw for lower surface of the wing......
plz send me some good reads about adding source terms using udf's i m also reading the UDF manual.
|All times are GMT -4. The time now is 16:09.|