# convergence for transient/steady state simulation

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 2, 2005, 10:51 convergence for transient/steady state simulation #1 Gab Guest   Posts: n/a 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

 August 2, 2005, 18:57 Re: convergence for transient/steady state simulat #2 Glenn Horrocks Guest   Posts: n/a 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 saha2122 likes this.

 August 2, 2005, 20:04 Re: convergence for transient/steady state simulat #3 Gab Guest   Posts: n/a 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

 August 3, 2005, 18:22 Re: convergence for transient/steady state simulat #4 Glenn Horrocks Guest   Posts: n/a 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

 August 4, 2005, 11:45 Re: convergence for transient/steady state simulat #5 Gab Guest   Posts: n/a Thanks, Glenn Best regards! Gab

 May 28, 2012, 14:59 #6 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 104 Rep Power: 8 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!!!

May 28, 2012, 18:46
#7
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
Quote:
 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.

 May 29, 2012, 07:58 #8 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 104 Rep Power: 8 Thanks Glenn But, when should we run it in transient??? Are "wiggles" a symptom, or reason to run problems in transient?

 May 29, 2012, 08:00 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,824 Rep Power: 85 This is all explained in the FAQ I linked to previously.

June 8, 2012, 01:35
#10
New Member

Join Date: Apr 2012
Location: Sydney, Australia
Posts: 10
Rep Power: 5
Quote:
 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.

 June 8, 2012, 01:42 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,824 Rep Power: 85 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).

August 14, 2012, 04:33
#12
Member

Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Quote:
 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

 August 14, 2012, 07:55 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,824 Rep Power: 85 Can you post some images of what you are seeing?

August 14, 2012, 08:26
#14
Member

Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Quote:
 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

August 14, 2012, 08:29
#15
Member

Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Quote:
 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

 August 14, 2012, 08:55 #16 Member   Mina Join Date: Apr 2011 Posts: 88 Rep Power: 6 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

 August 14, 2012, 19:12 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,824 Rep Power: 85 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.

 August 14, 2012, 19:27 #18 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 104 Rep Power: 8 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 likes this.

August 15, 2012, 04:04
#19
Member

Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Quote:
 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?

 August 15, 2012, 07:54 #20 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,824 Rep Power: 85 Can you post an image of what you are modelling and your CCL?

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post colopolo CFX 13 October 4, 2011 22:03 icemaniac178 CFX 1 March 30, 2011 19:11 Mansureh ANSYS 4 February 2, 2011 07:00 nuimlabib Main CFD Forum 6 October 2, 2009 15:03 Tomislav Main CFD Forum 1 December 6, 2006 08:53

All times are GMT -4. The time now is 19:30.

 Contact Us - CFD Online - Top