[Mina_Shahi]

Originally Posted by ghorrocks

Can you post an image of what you are modelling and your CCL?

this is the geometry i am dealing with:


Picture3.jpg

Picture2.jpg


i have two inlets: one is for ch4 (mass flow rate is defined) and one is for air (velocity is given)
i have outlet which is zero pressure
and finally nonslip adiabatic walls

the turbulence model is SST

[ghorrocks]

Your mesh does not look very good quality. You have massive jumps in element size and terrible aspect ratios. This mesh is going to give very inaccurate results. I would not trust any results from that mesh.

[juliom]

Dear Mina,
Can you share with us your mesh information, Quality, skewness etc.
I agree with Glenn, you have some jumps which will led you to some numerical problems.
Regards

[Mina_Shahi]

Originally Posted by ghorrocks

Your mesh does not look very good quality. You have massive jumps in element size and terrible aspect ratios. This mesh is going to give very inaccurate results. I would not trust any results from that mesh.

what can i do? i have very narrow space 3 mm and over there i need some elements, or in the fulel inlet i have 1 mm dimension , which i need some elements there ...

on the other hand if i want to keep the same dimension in other region then the mesh will be huge ...


and according to CFX solver when it first check the mesh : Aspect ratio is OK (17) (WITH CAPITAL LETTER WHICH MEANS IT IS VERY GOOD) Expansion factor is ok (15)(with small letter which means acceptable), orthogonality angle is ok (37)(with small letter which means acceptable) but for the unstructured mesh orthogonality angle is (!) (which means has problem)

and i don't know how to fix problem with orthogonality factor.

about skewness the min value (1e-5) and the average (0.2) are ok but the max is 0.99 which should be a bit less. (in unstructured mesh)

[Mina_Shahi]

Untitled.jpg


this shows that the quality of my mesh is ok at least for structured case.

[ghorrocks]

this shows that the quality of my mesh is ok at least for structured case.

If only it were that simple.....

Trust me, your structured mesh is terrible and it is making your results rubbish.

The CFX OK/ok/! categories are just guides and are not applicable to all simulations. Some simulations require high quality meshes, some are tolerant of lower quality meshes. Also these simple metrics do not capture all types of poor mesh quality.

what can i do? i have very narrow space 3 mm and over there i need some elements, or in the fulel inlet i have 1 mm dimension , which i need some elements there ...

Generating a quality mesh in difficult geometries is one of the very challenging (and often underestimated) skills required for a good CFD analysis. Practise, experience, training and lots of experimenting is requierd to generate quality meshes.

Can you post an image of the unstructured mesh?

[juliom]

Dear Mina, I don usually use the information from CFX solver. What I do is, I use the quality report from ICEM CFX.
From your case, I see one important thing, your skewness is to high. As I told you before. I have worked with unstructured mesh and I have gotten very good meshes with skewness bellow of 0.65, but in your case is 0.99. I think CFX recommends until 0.8. As Glenn said, I would not trust in the results you are getting from the solver

[Mina_Shahi]

Originally Posted by ghorrocks

If only it were that simple.....

Trust me, your structured mesh is terrible and it is making your results rubbish.

The CFX OK/ok/! categories are just guides and are not applicable to all simulations. Some simulations require high quality meshes, some are tolerant of lower quality meshes. Also these simple metrics do not capture all types of poor mesh quality.



Generating a quality mesh in difficult geometries is one of the very challenging (and often underestimated) skills required for a good CFD analysis. Practise, experience, training and lots of experimenting is requierd to generate quality meshes.

Can you post an image of the unstructured mesh?

Sure , but probably you would say the same for this one
becasue i already knew that the results by using this mesh are very bad

Untitled.jpg

[Mina_Shahi]

Originally Posted by juliom

Dear Mina, I don usually use the information from CFX solver. What I do is, I use the quality report from ICEM CFX.
From your case, I see one important thing, your skewness is to high. As I told you before. I have worked with unstructured mesh and I have gotten very good meshes with skewness bellow of 0.65, but in your case is 0.99. I think CFX recommends until 0.8. As Glenn said, I would not trust in the results you are getting from the solver

yes i know the maximum skewness is high for unstructured mesh, but not for structured grid. and ok ok Ok is what CFX solver gives me for structured.
for unstructured as i told before it shows (!)

[ghorrocks]

Sure , but probably you would say the same for this one

At that scale I cannot see anything wrong with it. But you need to look closer to be sure.

What I am looking for is the size of adjacent elements - there should be no large jump in element size, and the aspect ratioes should be reasonable - and any high aspect ratio element should be aligned with the flow.

From this view the unstructured mesh appears to have better transitions from fine to coarse mesh, and the aspect ratios of the elements is better. But you would need to look closer to be sure.

[Mina_Shahi]

Originally Posted by ghorrocks

At that scale I cannot see anything wrong with it. But you need to look closer to be sure.

What I am looking for is the size of adjacent elements - there should be no large jump in element size, and the aspect ratioes should be reasonable - and any high aspect ratio element should be aligned with the flow.

From this view the unstructured mesh appears to have better transitions from fine to coarse mesh, and the aspect ratios of the elements is better. But you would need to look closer to be sure.

Hi

i understood when i use inflation layer high-skewed cells and quality of mesh decreases while without inflation layer the quality is very good skewness is very low and ...
but without inflation i i am not able to resolve boundary layer, what do u suggest then?


another thing : i tried to use different mesh method i had skewness bellow of 0.65, orthogonality quality of higher than 0.4, the other parameters are also ok, no big jump (uniform mesh but not very fine) ...
it converged very fast no oscilation in convergence this time ,BUT still i have asymmetric velocity !!!!!!! what can be the reason then????? I used coarse but rather uniform mesh with all parameter in the good range. i didn't expect exact result but not asymmetric !!!

[ghorrocks]

i understood when i use inflation layer high-skewed cells and quality of mesh decreases while without inflation layer the quality is very good skewness is very low and ...
but without inflation i i am not able to resolve boundary layer, what do u suggest then?

Inflation is very important to accurately model boundary layers in mid to high Re flows. This will often give you high aspect ratio elements, but providing they are aligned with the wall (and thus the flow) they are OK. But even still, try to keep under an aspect ratio of about 100. Some flows can handle higher than this, some less - do a sensitivity analysis to determine in your case.

It is not impossible that the assymetric solution may well be correct. Do you have data which shows what the flow should look like?

[Mina_Shahi]

Originally Posted by ghorrocks

Inflation is very important to accurately model boundary layers in mid to high Re flows. This will often give you high aspect ratio elements, but providing they are aligned with the wall (and thus the flow) they are OK. But even still, try to keep under an aspect ratio of about 100. Some flows can handle higher than this, some less - do a sensitivity analysis to determine in your case.

It is not impossible that the assymetric solution may well be correct. Do you have data which shows what the flow should look like?

Thank you for the answer,

in the case of hot flow (with combustion) yrs but when it is cold no i don't think so

[ghorrocks]

Inflation layers are important if your flow has thin boundary layers which contribute significantly to the results. That boundary layer could be thermal or could be momentum. In a cold flow the thermal boundary layer is not important, but the momentum boundary layer might be. I cannot judge this based on the information you have supplied so far.

[Mina_Shahi]

Originally Posted by ghorrocks

Inflation layers are important if your flow has thin boundary layers which contribute significantly to the results. That boundary layer could be thermal or could be momentum. In a cold flow the thermal boundary layer is not important, but the momentum boundary layer might be. I cannot judge this based on the information you have supplied so far.

Yes that is true

what i meant from last post was that in the case of hot flow in reality we have unstable condition and flow may be asymmetric as well but in the case of cold flow i am not sure

i know having inflation layer is very important but taking them to account decrease the quality of mesh and i don't know how to fix this problem

[ghorrocks]

OK, as long as you see that it is quite possible the cold simulation is asymetric.

As for your second sentence, my post #26 said

Generating a quality mesh in difficult geometries is one of the very challenging (and often underestimated) skills required for a good CFD analysis. Practise, experience, training and lots of experimenting is requierd to generate quality meshes.

So all I can say is do all the meshing tutorials and training you can. Then try all the options on the mesher of relevance to see what they do, and run benchmark problems to find what is important for your mesh. There really is no other way, you just have to learn the tool to produce good meshes in complex geometries.

[Mina_Shahi]

Originally Posted by ghorrocks

OK, as long as you see that it is quite possible the cold simulation is asymetric.

As for your second sentence, my post #26 said


So all I can say is do all the meshing tutorials and training you can. Then try all the options on the mesher of relevance to see what they do, and run benchmark problems to find what is important for your mesh. There really is no other way, you just have to learn the tool to produce good meshes in complex geometries.

I hope i can get better results , thanks for all your answers