turbulent viscosity limited to viscosity ratio of 1.000000e+05

[Random86]

Good morning, everyone. I am a student of aerospace engineering and for the thesis I have to realize a model of bulb+derive for a sailboat more various fitting solutions.
I realized the mesh of the model with icem cfd; exploiting the symmetry of the problem I considered only half of the domain. Moreover, I imposed the transition from laminating to turbulent inserting a plan within the computing domain. as solutor use fluent.
the account is incomprehensible and stationary and has as objective the calculation of resistance and wall efforts (on the bulb and in particular in the connection zone). for this reason I also inserted a mesh of limit status ranging from 1 to 200 y+ to be able to use the enhanced wall treatment. the mesh is unstructured, with layer mesh limit to pentahedri ( prisms as it calls them icem) and then tetrahedri outside. Now, once the mesh in icem I checked it to verify that there are no errors, and in fact it does not return any error. So I went to fluent analysis. uploaded the mesh, I defined the model as k-eps feasible with enhanced wall treatment; I defined the speed in the inlet and a pressure condition on the outlet, while the plan inside the domain, which divides the laminar area from the turbulent one, I defined it as interior.
once I do this, when I launch the account (re=10^6), I get a warning message like:
turbulent viscosity limited to viscosity ratio of 1.000000e+05 in tot cells
where the number of cells varies with interaction. In addition, known that the residual of the continuity equation does not converge at all, but rather almost diverges, as the value of the resistance coefficient.
thinking that the problem was related to the separation of the domain in two I also tried to launch a completely turbulent account, but without any acceptable result.
I also get the same problem both that you work on a mesh of a million elements, and on a seven million and passes. Can anyone help me? ? ? ?
Thank you.

 

[Sylnet]

I think you've already tried. but did you try to put below lower relaxation values in the equations that give you problems? try from an upwind 1st order until convergence and then set an upwind 2°

 

[Sylnet]

if you find a solution could report it, I am also interested in this problem

thanks and good day

 

[Random86]

I'm working on it. Apparently it is mainly a problem of boundary conditions. I also tried to change the solutor from simple to coupled, and it seems to produce better solutions: in the sense that the eq. of continuity does not diverge, but in fact does not even give the impression of converging much. However I noticed that the number of cells that give the problem with this method is reduced and from a certain iteration then disappears. the problem is that the calculation times are long! So for now I am trying to find appropriate conditions to avoid using this scrum, although in the end I think that on the final account I will use this and I will wait patiently. As soon as I get new news, he'll let you know. Bye!

 

[Sylnet]

Have you tried with spalart allmaras to solve the turbulence equation? This method uses only one equation, so it turns out a little less accurate than k-eps but it is very used in aeronautics, because using models with many elements it is preferable to use simpler equations and therefore more read in the computational profile.

Perhaps by completely changing the pattern of turbulence the problem could improve greatly. cmq another cause of its error could be that it did not properly resize mesh when it was imported into fluent...but I assume that this has already verified it being a fairly common error

for the moment is everything, and wishes for the problem :smile:

 

[sail]

a high viscosity turbulent that then disappears can be given by cells with great aspect ratio (if hexa) or high skewness (if tet), together with a situation of great stress change compared to nitialization.

to accelerate convergence you can increase the underrelaxation of the turbulence intensity and dissipation at first, check that the turbulence intensity and dissipation rate of the inlet are realistic, visually check, after a few iterations, that the mesh is in place in the area where this high turbulence intensity develops, try with more flexible numerical patterns (simplec/simpler if incompressible).

other "trucchetti" consist in making a fast simulation with the same geometry but a more rational mesh (usually it is less sensitive to this problem because the cells are less stretched, especially in the bl) and use it as an initial condition for simulation with the thicker mesh.

between the top use second-order methods, if the simulation does not diverge, it definitely improves the speed of convergence. It is true that it is numeirically more challenging than the upwind1, but it is also less dissipative and generally uses a mino number of iterations.

random, out of curiosity where you study and for what kind of boat is the drift and bulb? Are they isolated or with hull and multiphase?

this and good luck

 

[Sylnet]

I agree that 2nd order upwind is less dissipative, but it is also less stable is at the risk of overshooting, even if they are limited! is not cmq better a first order that simply to determine the cell center uses properties on adjacent faces? The second-order overwind looks at two cells upstream and one downstream compared to the direction of the flow, so having very distorted elements as rightly she hypothesized, brings me a big inaccuracy in the calculation if you are using very distorted cells upstream and little distorted downstream...in the sense that I risk having too high value at the point where I want to get the calculated property.

My own were more than personal considerations, if I was wrong, let me know

Good day

 

[Random86]

random, out of curiosity where you study and for what kind of boat is the drift and bulb? Are they isolated or with hull and multiphase?

I'm studying at the Milan Polytechnic, aeronautical engineering. as reference I am considering the boats of tp52, which have as advantage the fact of not having winglets on the bulb and therefore a simpler geometry. Moreover I am not considering the hull, but only bulb and first part of the drift (in particular, I consider 3m of bulb and 3m of drift in model 1:1). this to limit the size of the domain and succeed in creating more limited mesh. the thesis continues in fact a previous work in which a study to potential+strate edge attack on the wake of the article of oudheusden, caspare and others, "attachment-line approach for design of wing-body leading_edge fairing". on a very small domain, which considered only a quarter of bulb (the upper half from the nose to the point of maximum thickness) and only a small part of drift.
now I should succeed and realize the simulation on a more extensive domain, even to check their results, especially for the potential approach+bl atac board.
I'm already using methods of the second order, but it doesn't change much. the only change I noticed was using the coupled scheme, although with obvious slowdowns.
I actually have a skewness problem in some areas. in particular on the exit edge of the drift. Now, I am exploiting the symmetry of the problem and therefore I consider only half bulb and drift. the exit edge of the drift is therefore adjacent to the symmetry plane. After the first problems on the models, I saw that skewness had problems especially in this area. I thought I'd cut the edge off. But they told me that the problem can only be solved by infitting the number of knots. However, with a proof that I had done, passing from 6 to 7 million elements, the problem cells passed from 11000 to 7000 and however the solution was not acceptable. Is it still appropriate to truncate the edge of the profile? Thanks for the advice. Bye!

 

[Sylnet]

mh... I don't know if I'd cut off the edge. It would be better to see the case in order to judge better. in my opinion I would leave it, it could generate vortices and gaps of the fluid vein that would affect the back of the bulb. Now I am not very practical of dynamic fluid boats on hulls, but going for a few years by boat I can tell you that it drifts over a certain speed often vibrates a lot, and it feels right on the boat, precisely because of its vortices. Would it be too big to fix mesh?

 

[Sylnet]

apart from what conditions did you use on the contour? a velocity inlet and a pressure outlet
while for other surfaces you used symmetry? What speed do you use for flow?
Monday I try to inform me

 

[Random86]

the problem related to reorganizing the mesh is related to the fact that with the pcs that the university gave me available I can not go up much in size yet. Maybe I can reach 9 million, but I still think the problem remains.
for boundary conditions:
- inlet: inlet-velocity with speed set at 17.894m/s;
- pressure-outlet;
- symmetry other 4 remaining surfaces.
the symmetry condition is critical, especially on the upper part of the box, where you have the intersection of the drift. However it was to avoid the problem of speed nothing I get by imposing wall -> no slip.

 

[Sylnet]

no bo I would have put the same conditions... I would do the mesh to reduce both skewness and the number of cells...in the sense that maybe it was not well done from the beginning mesh, so you could optimize it a little. It just doesn't mean you can get a skewness reduction. I would put a 3-4 mine to the max of cells, I would make a first simulation, and then through fluent there a function that allows you to adjust where you have a gradient of some high property, for example you can say that where you have a big li fluent speed gradient will have to do a mesh jam. I know that remaking mesh is a great workmanship but risk of wasting less time.

 

[sail]

I agree that 2nd order upwind is less dissipative, but it is also less stable is at the risk of overshooting, even if they are limited! is not cmq better a first order that simply to determine the cell center uses properties on adjacent faces? The second-order overwind looks at two cells upstream and one downstream compared to the direction of the flow, so having very distorted elements as rightly she hypothesized, brings me a big inaccuracy in the calculation if you are using very distorted cells upstream and little distorted downstream...in the sense that I risk having too high value at the point where I want to get the calculated property.

My own were more than personal considerations, if I was wrong, let me know

Good day

First of all let's say about you, otherwise I feel embarrassed. :tongue:

then, as I remember:

the problems of convergence, undershoot and overshoot should be own of the central difference schemes, which are second order but I referred to moments, k and epsilon, which are second order upwind. But obviously I can be wrong.

Also by memory it does not seem that an upwind scheme takes two cells upstream and one downstream but for the first order to the upstream face takes the value of the upstream cell, while for the downward face takes the value of the reference cell.

the second order upwind instead takes only the two stencil upstream.

But I reserve the right to change the answer after checking math:biggrin:

I'm studying at the Milan Polytechnic, aeronautical engineering. as reference I am considering the boats of tp52, which have as advantage the fact of not having winglets on the bulb and therefore a simpler geometry. Moreover I am not considering the hull, but only bulb and first part of the drift (in particular, I consider 3m of bulb and 3m of drift in model 1:1). this to limit the size of the domain and succeed in creating more limited mesh. the thesis continues in fact a previous work in which a study to potential+strate edge attack on the wake of the article of oudheusden, caspare and others, "attachment-line approach for design of wing-body leading_edge fairing". on a very small domain, which considered only a quarter of bulb (the upper half from the nose to the point of maximum thickness) and only a small part of drift.
now I should succeed and realize the simulation on a more extensive domain, even to check their results, especially for the potential approach+bl atac board.
I'm already using methods of the second order, but it doesn't change much. the only change I noticed was using the coupled scheme, although with obvious slowdowns.
I actually have a skewness problem in some areas. in particular on the exit edge of the drift. Now, I am exploiting the symmetry of the problem and therefore I consider only half bulb and drift. the exit edge of the drift is therefore adjacent to the symmetry plane. After the first problems on the models, I saw that skewness had problems especially in this area. I thought I'd cut the edge off. But they told me that the problem can only be solved by infitting the number of knots. However, with a proof that I had done, passing from 6 to 7 million elements, the problem cells passed from 11000 to 7000 and however the solution was not acceptable. Is it still appropriate to truncate the edge of the profile? Thanks for the advice. Bye!

beautiful tp 52! but do you also have experimental results? the trailing edge is always a little pain to manage. the best thing would be to do it round so that it closes on itself and the cells are belline, at the practical act, while it is true that it can vibrate, a steady ranse fail to grasp these phenomena, and recirculation would be so minimal to be infused at the practical act.

I feel like a lot of cells. to have an idea, how big is the domain? and the mesh of bulb surface and blade? on how many points does the bl mesh develop? I ask you because on a bohm paper and graph presented at the 18th chesapeake sailing yacht symposium we talk about mesh remarkably more rare, with a quite exoso turbulence model and without symmetry in half bulb. quarters and parolini instead, in the mox report 10-2007 they use 20 million cells, me also here without symmetry, and they had to kill winglets too.

 

[sail]

no bo I would have put the same conditions... I would do the mesh to reduce both skewness and the number of cells...in the sense that maybe it was not well done from the beginning mesh, so you could optimize it a little. It just doesn't mean you can get a skewness reduction. I would put a 3-4 mine to the max of cells, I would make a first simulation, and then through fluent there a function that allows you to adjust where you have a gradient of some high property, for example you can say that where you have a big li fluent speed gradient will have to do a mesh jam. I know that remaking mesh is a great workmanship but risk of wasting less time.

to be very happy. Meshatura is everything.

 

[Sylnet]

I checked, the 2nd-order upgrade only goes two cells upstream as you said....because I confused it with the quick (thanks a thousand! :smile, but in the algorithm there are limiters to avoid having too high values, which would not be real and consistent with the case.

for mesh also seems a little too thick, for that I proposed to remeshare properly but halving the number of elements. and then launch a simulation and see where there are still problems, and in those areas inflate using directly fluent

 

[sail]

There are limiters, but only gradients and I would expect, with a mesh "decent" and sufficent iterations of the gradients not huge in this case. Moreover it is not a compressible fluid with shock and rarefaction (this case the limits and the upwind spread the shock on 8 cells). Maybe on stress, but going to convergence should spread.. .

ot- have you then raised on how to calculate the load loss? fluent can calculate it accurately compared to "empirical" methods?

 

[Sylnet]

mh...you say there are limiters only for gradients? You mean I'm going to see the value of the gradient...it seemed more than it would compare the values between adjacent cells to decide whether or not to limit the value, and not to look at the gradient...in if with the gradient I don't know if the value I'm calculating is higher than the cells that are near me, I know if I calculate the property at a given point. But I might be wrong. I hope I've explained well!

cmq no, nn know well how to get the load loss between two floors directly in fluent...I think that looking at the static pressure on the faces, then the average I could get it...but the value didn't convince me much. If you know something I would thank you very much :biggrin:

 

[Random86]

but do you also have experimental results?

in the future yes, but lack funds to realize the model.. .
the mesh from 6 million elements develops on a domain that extends for 1m in front of the nose of the bulb and for 2.5 behind the bulb itself, with a lateral distance of .60m, as is of .60m the distance between the axis of the bulb and the bottom of the computing domain.
Now I was advised to consider a more extensive domain: 2m in front of the bulb and 4m behind, below and on the side.
the bulb has length 1m, as the drift.
on this mesh I consider a number of layer nodes limit that are about half the total, going from 1 y+ to 200.
I'm also led to try to reset the mesh, but I don't know where to go to parade. I could try to reduce the number of elements on the contour curves and refine the mesh on the body, but I don't think so by making mesh less large.

 

[Sylnet]

60 meters isn't too many? Now I don't know for the nautical as the field extends, but for cars or planes I usually took from 5/10 meters ahead to the object and 10/20 behind to let the flow develop well, this also avoids having flow reentries due to turbulence. Usually as you well know it is better to place inlet and outlet far enough, or melgio go where I do not have strong gradients for any property. While on the sides I don't know, I don't know, without seeing the project, I'd do 20 meters.

 

[sail]

in the future yes, but lack funds to realize the model.. .
the mesh from 6 million elements develops on a domain that extends for 1m in front of the nose of the bulb and for 2.5 behind the bulb itself, with a lateral distance of .60m, as is of .60m the distance between the axis of the bulb and the bottom of the computing domain.
Now I was advised to consider a more extensive domain: 2m in front of the bulb and 4m behind, below and on the side.
the bulb has length 1m, as the drift.
on this mesh I consider a number of layer nodes limit that are about half the total, going from 1 y+ to 200.
I'm also led to try to reset the mesh, but I don't know where to go to parade. I could try to reduce the number of elements on the contour curves and refine the mesh on the body, but I don't think so by making mesh less large.

the new dimensions have much more meaning (sylnet I think its .60 is to be understood as 0.60 m, too small) otherwise you risk that your solution is too influenced by the imposition of boundary condition.

Why don't you put some pictures of your mesh? Maybe we can give you more targeted advice.

As for the loss of load, I believe that making the difference of the integral surface of the pressures is the right process, but I wonder how accurate the cfd can be in these situations.
deep the loss of load in a straight pipe, if I don't remember badly is given only by friction, and here the cfd has some problemuccio (for example no one knows how to calculate the friction of a flat plate at high numbers of kings).