Hi, all

I am currently doing transient calculations because it's difficult to converge with steady state simulation for a multiphase modelling. If I run the problem as steady state, the best RMS I reach is 10^-2. After switching to transient model, it's very easy to reach 10^-5.

I have couple of questions here,

1. Can someone explain how to judge the convergence for a transient simulation? Should I run till RMS does not change significantly or just need to reach a certain RMS value as in steady state simulation

2. How can I check gas hold in my reactor in CFX-post with transient solution? Should I use a average value of many steps or simply just use the final step solution?

3. Theoritically, is it always correct to use transient solution to assist with convergence? I found it always very easy to meet the convergence criteria with transient simulation and the computation time does not increase.

I would appreciate your any input for my questions.

Best regards!

Gab

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

Hello, Glenn

Thank you very much for the answers.

In my case, I use the the transient flow fields(met the convergence level) as initial condition for tracer test simulation. Unfortunitely the tracer curve does not go smoothly. As from your comments, I think I may need to either run my transient solution for more steps till getting a stable solution, or use avergerage flow fields.

So, are there some easy tools in CFX-post or cfx-pre to get a average flow field over one or several steps?

Best regards!

Gab

Hi,

In CFX-Pre under the output options panel have a look at the "transient statistics" tab. That can give various statistical values, and using monitor points you can output values.

I don't know of anyway to generate an averaged flow field to view in CFX-Post, however. You could generate one using fortran or some post-processing I guess.

Regards, Glenn Horrocks

Thanks, Glenn

Best regards!

Gab

[juliom]

Dear all. I know this is a very old post, but I was reading the post and I found it very interesting.
I have a question, and I think that you have hada too.
Why when we have a steady problem convergence, people should say: he run it in transient and that`s it!!!
Why does it happen?
I know about the time marching method of ansys, but theoretically what is happeng withing the solver!!
thanks!!!

[ghorrocks]

Why when we have a steady problem convergence, people should say: he run it in transient and that`s it!!!

Not at all. Going to transient simulations is the option of last resort. This FAQ describes a more complete list of options: http://www.cfd-online.com/Wiki/Ansys...gence_criteria


If a flow is indeed transient then the steady state solver will have a hard time converging as there is no steady state solution. Then obviously you need to run transient to obtain convergence. But failure to converge in steady state can be caused by many factors other than this, so do not assume that all convergence issues are solved by transient simulations.

[juliom]

Thanks Glenn
But, when should we run it in transient???
Are "wiggles" a symptom, or reason to run problems in transient?

[ghorrocks]

This is all explained in the FAQ I linked to previously.

[MuhammadK]

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

Hi Glenn,

I had run my simulation, its a model structure inside a wind tunnel. It didn't converge, and I had a run with transient analysis. However, after running for a few days, it does not converge. What I had was;
total time = 2[s]
timesteps = 0.005 [s]

What could be possible source(s) of error?

Thanks.

Muhammad

[ghorrocks]

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).

[Mina_Shahi]

Originally Posted by ghorrocks

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).

Hi Glenn

I am simulating a mixing flow inside a chamber (with rectangular cross section) I used SST turbulence model for steady state simulation. and i used two king of mesh : structural and unstructured.
With the structural mesh i didn't have any problem in convergence , the residual decreased very smoothly while for the unstructured mesh it decreased to some level and then it start oscillating. so i changed the discritzation method from high resolution to upwind (after 100 iteration) and also changed the time step to very big value , then it converged to 1e-5. (while still had oscillation) . but My results show that the velocity profile in some sections are not symmetric with respect to the centerline and also the mass concentration of spices. i don't know what is the reason or how to explain these asymmetric results!!!
the results obtained from structured mesh are symmetric and changing the size of element didn't change the flow field that much.

I will appreciate any help from you.

Thank you
Mina

[ghorrocks]

Can you post some images of what you are seeing?

[Mina_Shahi]

Originally Posted by ghorrocks

Can you post some images of what you are seeing?

convergence of unstructured mesh .jpg

velocity at y 20.jpg


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

[Mina_Shahi]

Originally Posted by Mina_Shahi

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

structural residual.jpg

this figure shows the convergence of model by using structured mesh

[Mina_Shahi]

Dear Glenn

the graph i showed is relatet to the coarser mesh, but you can see assymetric behaviour for finer mesh as well you can see in this attached graph comparing the velocity profile for three different mesh sizes.

the assymetric behaviour is more clear for coarse mesh but it can be also seen for two other meshes as well.

to cfd online.jpg

[ghorrocks]

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.

[juliom]

Dear Mina,
Sometime it is not because of the mesh quality. I have had very good unstructured mesh, (Quality above 0.4 and skeness under 0.65).
With this quality of mesh it is almost sure you can get congervence with easy physics, but, regardless I do I have had never gotten convergence with some simualtions, for example, vertical separator, usign just air as "test".
There are a lot of information about this topic! and I would liek to know the real Why!!!
Regards
Julio M

[Mina_Shahi]

Originally Posted by ghorrocks

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.

Thanks for the answer,
But i don't think that it is just because of quality. the flow in really is unstable due to acoustic and if you monitor pressure inside the chamber you will see pressure velocity and ... are osculating. actually my geometry is a combustion chamber and and we have mixing of ch4 and air. and in this condition (special mass flow of air and ch4) we have unstable flame. so we have to also use combustion model but first i wanted to model the cold flow to see the effect of mesh.
this is pressure inside the chamber obtained from experiment:

DP_bottom_time.jpg


what i want to say is that this flow (even cold flow without combustion) is unstable, so i think this oscillation in residual of steady state calculation may come from that!!!!! but then the question is why it is not that clear in structured mesh. What do you think?

[ghorrocks]

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