Originally Posted by Glenn Horrocks
;72801

Hi,

To answer your questions: 1) The guide as to convergence level for transient simulations is the same as for steady state, in terms of RMS/MAX residuals and imbalances (if appropriate).

2) and 3) When you use a transient simulation to get what you believe is a steady state answer, what you are doing is physically advancing the flow in real time and letting the flow settle itself out. If the flow really is steady state then the simulation should steady out and every timestep is the same. If the flow is transient, then you will need to do some sort of averaging - if the flow is oscillatory (eg a vortex street) then averaging over a cycle or two should be OK, but if it is chaotic (eg LES simulation) you will need to do some homework and determine what is the longest important timescale and make sure you include that. Obviously if the final flow is transient you cannot use the final timestep flowfield alone to represent the "averaged" flowfield, but you need some sort or average over an appropriate timescale.

You will almost always get individual timesteps to converge when you use a transient simulation - you just need to get the time steps small enough. However, to get a useful answer you will usually need to do many timesteps until the result does not change between timesteps.

Regards, Glenn Horrocks

Originally Posted by ghorrocks (Post 365373)

My post from seven years ago tells you exactly what to do - you need smaller time steps (assuming the basic setup of the simulation is correct).

Originally Posted by ghorrocks (Post 377018)

Can you post some images of what you are seeing?

Originally Posted by Mina_Shahi (Post 377028)

Attachment 15161

Attachment 15160


after 100 iteration you can see a sudden change this is because of changing from upwind to high resolution scheme . as i mentioned with high resolution i didn't have convergence so i first start with upwind and then switch to high resolution and then increased the time step.

thank you

Originally Posted by ghorrocks (Post 377119)

It appears your unstructured mesh is of a low enough quality that is making convergence harder than the structured mesh (which appears to have a higher mesh quality). This is also leading to other problems such as a non-physical assymetry.

Originally Posted by ghorrocks (Post 377195)

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

Originally Posted by ghorrocks (Post 377276)

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.

Originally Posted by ghorrocks (Post 377355)

:) 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?

Originally Posted by juliom (Post 377356)

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

Originally Posted by ghorrocks (Post 377424)

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.

Originally Posted by ghorrocks (Post 377707)

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?

Originally Posted by ghorrocks (Post 377728)

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.

Originally Posted by ghorrocks (Post 377757)

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.