I have a trouble in my simulations when I start the iteration after few seconds this message appear to me : turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 102 cells ? how can I fix this problem and what the things cause it?

Regards k.baker

Hi

This is due to either a bad mesh or inacurrate properties.

Regards

AAA

thanks for the reply. If the reson from the mesh how can i be sure about this? is there any way?

Thanks a lot k.baker

Hi

Try Adaption based on Gradients of Velocity. This should take care of it after few iterations.

Regards

AAA

I know about adapt gradient but where I should adapt the gradient for velocity (I donnot know which region that need adaption to overcome the problem) can you clear this point with more details ?

k.baker

Hey,

woul recommend you to first let it do a couple of 100 iterations. sometimes that message dissapears.

if it doesnt, you can do: adapt - gradient

then you click on -refine -gradient

then you can choose for example turbulence and turbulence viscosity ratio in the right panel.

for the treshhold you have to fill for example 100 in en then do 'mark' it's gonna tell you how much cells will be refined. then you can do refine (and click ok on hanging cell node..)

next you can see in the fluent window how much new cells you got. next you do iterate...

ps: fluent chooses the cells who have to be refined: the cells where there are big gradients..

greetz

salam ebrahim: I tried adapt gradient for turbulence viscosity ratio for threshold =100 then select mark and adapt as you mentioned but the problem aggravated and this appeared also from increasing the values of residuals to 10e+06 inspite I used very small under relaxation factors (nearly 0.01 to all variables) so what happen can you tell me? Another thing I want to ask how can I select the optimum value for refine threshold (I chose it 100 ) can you tell me please?

k.baker

it is trial and error..

you have to try a number and see what it gives.

when u have for example 10^6 cells, and when you want to refine it gives you 1000 cells to refine, then in most cases it won't to much.

try to refine your grid with 30% (so from 1 million to 1.3)

if you haven't got too much cells (like 300 000), you can double the number of cells, or just remesh your geometry.

it is also possible that the quality of your mesh is bad (skewness>0.97 or close to..) than you will have to remesh.

greetz

hey again : thanks for the response. I still need more explaining hope not bother you with it: 1) when selecting adapt >gradient under option should I select both of refine & coarsen or one of it? 2) when I chose gradient of turbulent viscosity ratio and press compute it give me Min. = 0.01074611 & Max. = 1899261 hence how much the number of refine threshold as you think? 3) I read the quality of mesh can be found from examine mesh option in gambit but it not shown to me the quality of equisize skew in spite I select range for display type and quality for display mode can you tell me how I do that?

Thanks a lot k.baker

in gambit: examine mesh, select range, see that your mesh is selected. and then select 'show worst element' it will give you the skewness. normally gambit alerts you when u have meshed a volume, that skewness is exceeded 0.97.

You should only select refine. Coarsen is when you have too much cells and your mesh is too fine.

tell me, how much cells do you have? when u do treshhold 100 what does it give when u slect MARK? when you do treshold 50 what does it give when u slect MARK? when you do treshold 20 what does it give when u slect MARK?

greetz

I have 38040 hexahedral cells my cylinder has 50 mm diameter and 16 m long. I not sure if the number of nodes is sufficient for this dimensions or no however I examined the mesh as you told me fluent wrote to me the quality equal to 0.516872 so is this value fine? when I set threshhold as 100 and select mark fluent type this message: 16491 cells marked for refinement, 0 cells marked for coarsening and when I press adapt hanging node this message appear: Dump usage: 38040 cells, 117034 faces, 41053 nodes

Dump usage: 38040 cells, 117034 faces, 41053 nodes

Dump usage: 153477 cells, 479116 faces, 172434 nodes

turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 816 cells

Grid size ( original / adapted / change)

cells ( 38040 / 153477 / 115437)

faces ( 117034 / 479116 / 362082)

nodes ( 41053 / 172434 / 131381)

so please tell me your suggestions.

hey, now i see.

I took 1/16 of your geometry, so i took 1m. (diameter 50mm)

I meshed it in gambit wit hex/wedge cooper, size 5, and i got 18156 elements. for the whole geometry, that's roughly 290 496 cells.

but in my opinion that is not fine enough (you have to see ur face mesh on the inlet of the cylinder) and you are not even close to that with 38 000 cells.

take size 3 or 4 and try again.

if it gives problems, then try to refine. but i think it would be okay whit a fine mesh.

I forgot to mention 38040 for just one half of the cylinder because I draw it as symmetric along the y-axis. Another thing i draw this mesh at first by drawing half circle (face) then mesh it with map after creating of a boundary layer then I sweep this face to create the whole volume with mesh too. Hence At the inlet the number of mesh is equal to 634 cell and the zones appeared in fluent as bellow:

38040 hexahedral cells, zone 2, binary.

38040 cell partition ids, zone 2, 2 partitions, binary. 111206 quadrilateral interior faces, zone 8, binary.

2160 quadrilateral wall faces, zone 3, binary.

634 quadrilateral pressure-outlet faces, zone 4, binary.

2400 quadrilateral symmetry faces, zone 6, binary.

634 quadrilateral velocity-inlet faces, zone 5, binary.

41053 nodes, binary.

41053 node flags, binary.

what you say about my procedure is it fine I want know your opinion and thanks a lot again.

38040 x 2 = 76 080 it seems not a fine mesh to me..

but hey, i see that you are using a pressure outlet.

i think you can use an outflow boundary condition. becaus your length is big, so your velocity prfoile is fully developed.

i had this problem too once. with a pressure outlet i got that error of viscosity.

so conclusion: -try outflow -if not, try to refine in gambit

Yes that's true I have fully developed flow but I am afraid outflow boundary may cause reverse flow but the question is this boundary work with the VOF multiphase flow model? if it work i will try it? can you please post me your email address into my email khalidb77@yahoo.co.uk i will try send you the mesh file.

dont know with the VOF model. you'l have to look it up in Fluent manual.

sorry dude, I haven't got time to look in your mesh file. My pc is constantly running on Fluent.

good luck

well only one thing remaining I checked the skewness to my mesh by examine mesh its equal to 0.516872 did you think this good quality or no?

Thanks

yes, skewness of zero is perfect mesh.

0.97 is very bad

everything smaller than 097 is ok, the closer to 0, the better. 0.5 is very good.

Hi

Try not to exceed a skewness of 0.4 and 0.8 for 2D and 3D simulations, respectively.

Regards

AAA

hey AAA I think there is confusing in your note and what mentioned in the manual because it mentioned that the excelent mesh obtained when the skweness factor being too small (equal zero) but this for 3D not know about 2D?