Discussion Forum

Yes you are right.
I too did that.
I am getting results no way matching with the theory. It is surprising despite Re is very low and flow is steady and symmetric. I tried with wider fluid outer boundary, laminar inflow BC, creeping flow, direct, iterative solver approaches all giving values no way closer to the theory.

I used reacf(u) and (v) for force calculation over boundary and used reacf(u)/( ρdU^2), for drag coefficient calculation.

It is surprising why such huge difference between theory and comsol? Someone will look into the attached file? I have attached theoritcal results and my comsol file. Please some one help us.....

Hi

First of all you should update your version to the latest patch
then I'm astonished you are not using the default "physics induced" mesh, it proposes a boundary layer around your "ellipse wing" and that should give better results, perhaps with a extremely fine settings on teh boundary, as your volume is very large compared to the ellipse. but you can also set the boundary layer manually, without I'm not astonished that your results differ.

Last thing you say nothing about your fluid, or if its the one of the tables

--
Good luck
Ivar

Thanks Dr. Ivar
I did that too.
The results are same in 4.2 a and with physics controlled mesh, I also checked boundary layer both automatic and manual with '8' layers returned same.
The fluid is 'user-defined' as given in the parameter values rho1 and mu1.
Please help me dr.Ivar,
I dont know how to get that theory values.

Thanks again for your suggestions.

Hi

I cannot really do much, I believe, so long your results varies with the mesh density, you are not really in a steady state situation and your estimations of Cd and Cl will be rather wrong, whatever you do.

Anyhow, I have some difficulties to accept your Re formula in the Parameters section, the 2*L*f seems very suspicious, your characteristic length is rather 2*b or there around.
Then from your Derived Values why reacf(u)^2/rho/U^2 the dimensions does not seem correct. Reacf(u) in CFD has units of [Pa] (these are still missing, you need to define them by hand), integrated over the chord one remain with [N/m], multiplied per 1[m] default "d" model depth you get [N]

Take care too the "Cell Reynolds" number of COMSOL is not the standard CFD Reynolds number, it is reported to the mesh size "h" and not the true geometry sizes, and used for mesh density check
Many of these dimensionless CFD variables depend on a characteristic length or area and this L and A values introduces some guess work. therefore I cannot be sure you can compare correctly your table values and the one from COMSOL like that

--
Good luck
Ivar

Thanks a lot Dr. Ivar.

I have used Young's definition of Reynolds number using non-dimensional characteristic lengths. He calculated Reynolds number based on the major axis of ellipse and non-dimensionalised by Re = (2 Ud cosh ξ /ν) where tanξ = b/a. I calculated this through that 'f' in that paramater table. Moreover I calculated drag coefficient using Cd or Cl = lineintegral of the boundary : reacf(u or v)/(rho1.L*U^2). Please see the picture attached from that reference.

Actully i did a complicated study using the ellipse and want to validate using this 'theory' it is not giving same value.

I really appreciate your patient in explaining this novice user.

With lots of regards
Shiphys

Hi

as you did not use full equations in your model it is not easy to follow. Anyhow here too the "L" and "D" are "nominal lengths" that needs some interpretation. Then you could use material properties closer to "air" if that is the medium, not that really it changes that much, if you adapt all parameters coherently, but it's easier for us out here to understand

At least use a fine mesh and a reasonable area around, and after the flow, normally COMSOL calculates quite correctly ;)

--
Good luck
Ivar

Thanks a lot for sharing your thoughts and feeding this novice.

I redid everything in 4.2a. physics controlled fine mesh, glycerol as built-in liquid, with all parameter table described. for this zero angle of attack and Re= 20, I should get Cd = 1·169 or at least 1·228. But I am getting 2.5843.

Any advice please...

Hi,
I notice in fully coupled solver you set the iteration or tolerance to 25,
if you only want a line integration to 1.88
i set it as 5. and get 1.86,

not sure if there is what you want.

Thanks Chiwei.
Doing that certainly changes the value. But when I check for other angles of attack (even with finer mesh), the results are different from theoretical results.
No clue what to do to get consistent results....

Hi

I would change 2-3 things, first for the wing,

why not use no-slip wall conditions (moving wall with velocity = 0 is the same as no-slip) ? $

then your upper/lower outer walls, to avoid a parabolic velocity profile, and to make the medium "infinite", you can use a symmetry boundary condition or a slip one, or even an "open boundary", all three will influence your results

you could also move the rectangle 5 units to the right to get the full velocity drop/recover view

Now from my understanding I would rather use "b" than "a" for the Re number (but I'm not that a CFD specialist, for me the drag constant is rather linked to the cross section and not first of all to the length. For your drag factor calculations, there is also a factor "2" in the flow energy, but it might cancel out with the "a" as it makes a/2

What I often like is to use a polar plot to see the sear components:
add a polar plot node, add a line graph node to the polar plot, Theta angle Parameter use expression and type atan2(y,x) (instead of spf.U), select you "ellps" for the 4 boundaries, and select the pressure p. then to improve the reading, in Color and Style, select width "2" and line marker "Cycle", add a legend, select manual and type "p (Pa)" (it's not automatic).
Then duplicate 4 times the line node and replace the variable and the legend respectively by: spf.K_stressx , spf.K_stressy , spf.T_stressx, spf.T_stressy.
Note the reacf(u) will not be easy to interpret, as its only defined on the nodes

Ideally one should make the same plot but for a shape slightly "inside the fluid", that can be obtained by adding an internal fluid boundary at 10% about greater size than the solid ellipse

Finally I would hesitate to use the extremely fine mesh for this case ;)


--
Good luck
Ivar

Thanks Dr. Ivar.
Please accept our appreciations from newbies. This is another instance how you actually mentor us elaborately by covering all related issues and taking up to the depths of CFD. A thread which could have been a normal one is filled with your teachings. Boundary conditions(slip wall removes parabolic profile and provides infinite domain=one has to spend hours/pages of readings of texts book to get this info), mesh settings, polar plots...more than CFD we want to 'dig' your knowledge and enjoy learning.

Regarding Re of elliptical cylinders:
The charect. length is taken differently by different authors, some take minor axis, some major axis and some equate the area of ellipse to circle and find the equivavalent dia to take as charect. length. But however, if we take Re defined as in the paper, should't we get matching results?- irrespective of the way how we measure Re.

I think still there seem to be big difference in results....
for your perusal I have attached the paper.

Hi

indeed the article is nice and interesting. As usual these theoreticians, use dimensionless values all over, so going back to "dimensonal" ones can be tricky, and anyhow, even if they make a scaling error the demonstration remains valid, it's us the engineers and practicians that have problems to get these theories to fit with our surrounding world.

You have a few choices, you can run COMSOL dimensionelss too, but I find it far to easy to do stupid scaling errors that are difficult to identify, up to you ;)

But, you should start to check that you are using the COMSOL CFD equations as equation (1) as stated in the abstract: they solve "Navier Stoces for incompressible fluids", as the CFD of COMSOL has different sub categories (see the main physics node, and track the changes in the equations and dependent variables.

Then check the dependent variables (you need (u,v)[m/s] and p[Pa]) and you have the parameter "R" that depends on constants U [m/s], d[m] and eta [m^2/s]. I agree here they define the dimension "d" as the major axis, so let^s use that to dimension U.

When you are changing the fluid you act on "rho" & "eta" the fluid density and respectively dynamic viscosity, but rho appears, as normalisation, also in Cd and Cl, as well for the pressure normalisation via the cinetic energy density of the fluid: 1/2*rho*U^2.

What I suspect is that by choosing glycerine and playing with the equations, you are using part of the dimensionless values and part of the dimensioned values of the equation of your article. This could imply a scaling error, also on Cd and Cl.

One "lazy engineering" approach, is to repeat the sequence of measurements done in the article (angle scan for a given Re), then compare the Cd & CL values and see if they happen to differ by a constant scaling value, this value, and the equations in the article should give you an indication what could differ (it could even be an error in the article, that happens, still rather rare ;)

Another point is that the article dscribes an integration on a closed contour inside the fluid, surrounding the ellipse shape, while COMSOL calculates the reaction foces on the fixed boundary. There you have the option in COMSOL to either add one or several "internal boundaries" surrounding the ellipse, but insde the fluid, if these are correctly resolved with the mesh you can integrate different values along thee boundaries, as for the article (you can use an ellipse at a given distance from the bondary, or simply a circle) but you can also define a parametric circle from the data set (this interpolates the domain values onto the contour). Note that COMSOL defines certain variables only on boundaries, so you get different results pre-defined if you use an interiour boundary, or if you use the Data set method.

Try it out, one need to play detective, when trying to fit theoretical results onto practical examples, the match is not always that obvious. But normally both methods should coincide, once correctly set-up ;)

And a last thing, the article shows vortex shedding for large angles, I'm not sure you can get that running like that in laminar with COMSOL, but that is outside my usual expertise, I'm not CFD expert ;) I'm learning as you are, its an interesting exercice.

--
Good luck
Ivar

Thanks again Dr. Ivar for a detailed and point to point explanation.
I am reading and applying your thoughts.

I have managed some of them (like mesh: normal, fine and finer, BC: slip, open and symmetry). I have compared them with the theory and attached in the picture.

It makes some sense now and I am able to understand the situation.
though there is difference, is it negligible?, is't the comsol algorithm is superior to the one in the paper?
I should have compared with experimental results, but in 2D I wonder are there any such validation from experiments.


With regards,
Siva

Hi

well what is the ratio between BC out symmetry with extremely fine mesh and the theory ?

something like 1.6/1.2 = 1.33

But that not far off from your selected "rho" w.r.t "1" or 1000 kg/m^3 which is a usual normalisation value often used for "rho".

Could that be an issue, missing a normalisation w.r.t. physical dimensional "rho" somewhere ?


--
Good luck
Ivar

Hi. thanks again.
Yes. BC outer: symmetry and slip wall gives almost same shape of curve as in theory only they are 0.4 units away uniformly. should I have to add this anywhere to get in agreement with theory? wont it change the outputs again...

Just out of curiosity, made the fluid domain bigger and bigger till i get the matching value...and got too for a very big rectangle around ellipse. Is this approach physically meaningful or just a trick ;-)

Hi

not necessarily. But if your mesh remains fine enough (doubling mesh size gives just a few % changes) then you should be mesh independent, then the effect you observe could indeed indicate that you do not have "infinite" enough distance between the "wall" and the wing.

You could try with an "open boundary" instead of "symmetric" one , the former will free the flow in and out, the latter force a parallel flow.
Or perhaps integrate the pressure and drag on the symmetric wall, if its not influencing the wing it should have values independent of the wing orientation

And as you are using glycerine you should check the dynamic viscosity [m^2/s] and the overall transverse (heigh) dimensions of your system.

Indeed many things to learn, and it's more fun with COMSOL as it's easy to test out the physics

--
Good luck
Ivar