[Shomaz ul Haq]

Dear all. Hope all are doing well. I have developed a model for counter flow double pipe heat exchanger with hot water inside and cold water outside. Even though all my values converge to a variable value less than 10^-4 within forty iterations I am getting oscillations from the start to end. I have checked the mesh. In fact when I changed the relevance center in mesh from medium to fine, only then I got convergence as my solution was not converging previously. Can anybody help how to fix this problem I went to the FAQs on solver related problems. It was stated to increase physical time step. Can anybody tell me how to get the residence time in CFX-Post by placing a streamline and looking at the Time variable on it to get the maximum value?" Also would this solve the problem. Would be extremely grateful. Thanks.

[Red Ember]

Shomaz, what timescale option do you use and how do you calculate time step (if you use physical time step)?
And what's about maximum residuals comparing to RMS?

[Shomaz ul Haq]

Thanks for the reply Red Ember. I am using Physical Timescale of 2 [s] in Timescale Control in Fluid Timescale Control. For Solid Timescale Control I am using Solid Timescale as Auto Timescale. I am also attaching jpegs for both residuals for heat transfer. Would be grateful for your help. Thanks

[Red Ember]

Both pics represent max residuals if my browser works correctly
Why 2 seconds, how you estimated it?

[Shomaz ul Haq]

Sorry about that. I have attached RMS residuals as well. I have two seconds as a guess. In your opinion what value should I take? Thanks.

[Red Ember]

1. Due to max/rms reiduals grid doesn't provide local convergence problems. Mesh is adequate.
2. Physical timestep seems too big according to view of residuals plot. Try to set it PT = (pipe diameter)/(average velocity)
3. I was told that Solid Timescale should not be automatic, although I can't recommend its value right now.
4. What about domain imbalances and monitor points?

[ghorrocks]

For CHT simulations you really should use imbalances as a convergence criteria. I bet if you look at your imbalances they are nowhere near converged.

For solid time scale factor you can normally use very big numbers - 100, 1000, even more at times. As the solid heat transfer equations are very numerically stable they can generally handle a large amount of acceleration, and the will accelerate the convergence of the imbalances a great deal.

[Shomaz ul Haq]

Thanks a lot Glenn. You are right for CHT problems imbalances reflect a good convergence criteria and my imbalances are not converging. Red Ember what diameter should I use, inner pipe diameter or annulus equivalent diameter? I know its a lame question but just want to confirm shouldn't I use annulus equivalent diameter of pipe? Would be grateful for answers. Thanks.

[Shomaz ul Haq]

Also isn't it stated to use a larger physical timestep in case of non convergence. What you are saying Red Ember is to use a small physical timestep. When I used physical timestep=(equivalent diameter)/(average velocity) and solid timescale as auto, heat transfer parameters were stable and straight wrt. accumulated timestep and did not converge within the full limit of iterations of 100. When I was using a value of 2 [s] for fluid at least values were converging even though with oscillations. I am confused what to do. Glenn and Red Ember please guide. Thanks.

[ghorrocks]

I would not be too precious about setting the time step size for a steady state run. Red Ember's is one approach, there are others (such as average residence time, or a representative dimension divided by a representative velocity).

In my experience you start with one of these estimates, any one, it does not matter much - but then you watch the convergence. If it is converging nicely but slowly you increase the time step size. If it is erratic and jumping about you decrease the size. If it is doing periodic hops you increase it by a large amount (x10 or so).

So you start with a rough estimate and you fine tune it from there. That is why the initial estimate does not matter much.

By the way: you change it with edit run in progress so you do not have to restart.

[Shomaz ul Haq]

Thanks Glenn. I used equivalent diameter of pipe for cold domain in calculation of PT. Is that okay? and what do you mean by "you change it with edit run in progress so you do not have to restart"? What do I change and how? Thanks.

[ghorrocks]

Let me quote it:

the initial estimate does not matter much.

Use any initial time step estimate you like, a reasonable guess will help, but just about anything will work. In solver manager under tools is edit run in progress. This option is available when the simulation is progressing.

[Shomaz ul Haq]

Thanks a lot Glenn. Understood what you mean't. I can edit solver control parameters while solver is running. I didn't know about this. That is great. So when I change a value while solver is running will the solver restart from start or start from that iteration where I changed solver control parameter? Also while watching convergence do I change physical timestep for fluid if solution is not converging, for solid or for both fluid and solid? I hope you understand what I mean. Thanks.

[ghorrocks]

Try it and find out.

The solver keeps running with the changed parameter. It does not restart.

[Shomaz ul Haq]

Also no matter what I do "Mass and Momentum 1" for Cold water domain oscillate a lot but converge quickly no matter what PT I use for fluid. Even though my parameter of interest are of heat transfer I would like "Mass and Momentum 1" to also converge. That is also bothering me. If my parameters of interest are not changing does one need to change PT in "Convergence Control" or in "Equation Class" for that particular equation that is not converging? Would be grateful. Thanks.

[ghorrocks]

This is an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria