CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)

 Kushagra June 19, 2008 22:11

Hello, It may not sound a serious question, but I still need to clear my doubt.

If I run the same simulation in steady state solver and transient solver, and somehow I manage the simulation to converge in steady state solver.

Will the result from both the simulations almost same? I could only manage the steady state simulation to converge by playing around the false time step.

Thanks so much, Kushagra

 cfd.newbie June 20, 2008 21:06

No, we expect more accuracy from transient simulation because it is time marching solution. I am very new to CFD though, it will be interesting if more experienced CFD user can give us insight into this.

Regards

 Glenn Horrocks June 22, 2008 19:51

Hi,

The difference between a steady state simulation and marching a transient solution to steady state is that the SS simulation ignores many of the cross terms and higher order terms dealing with time. These terms all go to zero in steady state so they don't affect the steady state result. The transient simulation includes all these terms. Usually this means the steady state model has an easier convergence as there are less terms to model and some transient non-linearities are removed, but in a few models these non-linearities help convergence (but this is infrequent).

Glenn Horrocks

 Kushagra July 3, 2008 00:25

Thanks Glenn for providing useful knowledge about convergence in both type of simulations. But what about quality of results from two type of simulations? Some time steady state simulations are difficult to converge but reducing the false time step by 1 or 2 order, they converge. Does it affect the quality of results?

 Glenn Horrocks July 3, 2008 02:55

Hi,

A fully converged simulation, run to steady state by either steady state or transient approaches should be the same. The only exception is when "local timescale factor" is used in a steady state run as it can accelerate convergence nicely but as different timescales are used across the domain can cause accuracy problems. As long as a steady state run is run to final convergence with a physical timescale (including auto timescale) then it should be fine.

The timescale is a steady state simulation is like under-relaxation from SIMPLE based solvers. Too high a URF and the simulation diverges, too low and convergence is slow, so you try to fiddle until you get the optimum in the middle somewhere.

Glenn Horrocks

 Kushagra July 3, 2008 23:50

Thanks so much Glenn.

1) So reducing the 'false time step' is similar to reducing the under-relaxation factor. (Or is it just opposite?)

2) Suppose the residual for Volume Fractions are not getting low and fluctuating around mean values, what should the user try first? Reducing or increasing the 'false time step'?

3) The residence time (volume of domain / flow rate) is 13 second for my multiphase case. what might be a good time scale to start with steady state problem.

Meanwhile, I found some of your, Robin's, Cyclone's replies on this forum about how the steady state solver works. They were really helpful.

Thanks, Kushagra

 Glenn Horrocks July 6, 2008 23:41

Hi,

1) Be careful thinking of the physical timestep size as a false timestep. False timestepping is a different technique used in SIMPLE based solvers (I think). In CFX, a steady state solver is similar to the transient solver, just with some higher order transient stuff and cross terms removed, and a different residual calculation.

But in basic idea, yes, tuning the URF of a SIMPLE run is similar to tuning the timestep size of a CFX run. There will be an optimum value somewhere between too slow and unstable.

2) http://www.cfd-online.com/Wiki/Ansys...gence_criteria

3) A good starting point is 13 seconds.

Glenn Horrocks

 cysanghavi July 11, 2016 11:27

Transient and SS !

Hello,
A basic conceptual doubt:
I am performning a conjugate heat transfer problem for a drilling process.
Lets assume, I want to see the temperature profile of the tool after 30s..
I have a tool fixed at intial temp. (lets say 600K). It loses heat by conduction and convection to the surrounding air. (radiation losses are neglected).
I will perform a transient analysis setting appropriate time steps..
Will this result be the same as a steady state simulation freezed at 30s. ?
(is this possible in CFX? Can i set it up the steady state simulation directly from 30s.)

I would say, it wont be the same because of:
1. Hconv is proportional to delta T which is proportional to time. (different tempertures at different time steps).
2. the conduction equation is a parabolic PDE, which has time. so the heat loss due to conduction is different at different time steps.

 Opaque July 11, 2016 12:25

If the transient calculation reaches steady state before 30 [s], say the transient contribution is already negligible at that time, the solution on the same mesh should be identical for a linear set of differential equations. For a non-linear system, there will only be identical if the system has one stationary solution.

If the time to reach steady solution is larger than 30 [s], the transient solution will be very different than the steady solution.

Summary: in general, they are very different unless you already know the "steady state time".

Hope the above helps,

 cysanghavi July 11, 2016 12:40

Lets say, I know the time when I achieve steady state.Lets say this time is 120 [s].
( I assume I achieve steady state, when there is no change in heat trasnfer, momemtum trasnfer.... etc. with time for the same mesh.)
At this instance, will my transient and steady state simulation yield the same results ?
the fact is that I do not understand how CFX evaluates the steady state solution.

 Opaque July 11, 2016 13:30

At this point, you are better off reading the ANSYS CFX documentation on how either analysis is carried out, as well as reading a book on partial differential equations.

If your application is purely heat transfer, a heat transfer textbook usually cover heat conduction on both steady and transient modes. I would not worry much about the momentum equation since the concepts are unique.

 cysanghavi July 11, 2016 19:44

2 Attachment(s)
Thanks for the references.
All I could find in the literature of CFX was the following informtion. photosAttachment 49054.
Attachment 49055.

I have the solver guide and the CFX Pre guide.
I do not know if there is some other literature that I can review. I searched various portals.
Could you refer me some literature, about equations that are solved for steady state ?

 Sasquatch August 16, 2016 08:29

Quote:
 Originally Posted by Glenn Horrocks ;88525 Hi, The difference between a steady state simulation and marching a transient solution to steady state is that the SS simulation ignores many of the cross terms and higher order terms dealing with time. These terms all go to zero in steady state so they don't affect the steady state result. The transient simulation includes all these terms. Usually this means the steady state model has an easier convergence as there are less terms to model and some transient non-linearities are removed, but in a few models these non-linearities help convergence (but this is infrequent). Glenn Horrocks

Dear Glenn,

I have tried to find out what are these "cross terms" but I didn't manage to find the good answer. Could you please explain what did you mean by this?

Best regards,

 ghorrocks August 16, 2016 09:23

I vaguely recall that there are some neglected cross terms but I cannot find any reference to it or recall much about it. Bruno's comment here (http://www.cfd-online.com/Forums/cfx...transient.html) says there is no difference except in the way the coefficients are updated in the iterations. There are also differences in the way the residual is calculated.

So I am not sure about the cross terms. But the updating of the coefficients and residuals are certainly different.

 Sasquatch August 16, 2016 09:48

Dear Glenn,

thank you for the reply, yes indeed, there is a difference in the way the RMS is computed, I have tried to find it in the documentation but I have not managed yet.

As far as I know, for SS it is:
RMS = |

where the N is the number of elements.

Do you know maybe whether it is treated in the Ansys documentation? Specifically for the transient case. I would like to find out more on this topic.

Best regards,

 ghorrocks August 16, 2016 20:51

Yes, that is the standard definition of RMS. The residuals are defined in section 11.2.3 in the theory guide. The definition is not thorough, but enough to get the idea. It also defines the difference between SS and transient.

 cleoo September 21, 2016 10:22

Quote:
 Originally Posted by Glenn Horrocks ;88525 but in a few models these non-linearities help convergence (but this is infrequent).
for which models does it help convrgence?

 ghorrocks September 21, 2016 19:55

I have changed my opinion on this since 2008. I use it much more often these days.

The main simulations where it makes a difference are things with complex coupling between equations, such as multiphase or shock waves, or where there is transient vortex shedding (which implies the simulation was not steady state in the first place).

 cleoo September 22, 2016 17:28

Hi Glenn,
Just a follow up, do you think that if you modeled a steady state case (where you knew was suppose to be a steady state case) with a transient one there should be no problem as they should theoretically yield the same result if it was truly a steady state case?

 ghorrocks September 22, 2016 19:46

Yes, the transient simulation should converge over time to the steady state case.

 vigneshz259 May 9, 2017 05:57

Can any tell me please what is the boundary condition in ansys icepak.

I'm doing thermal analysis of heat sink with three module .in the cabinet two side opening one side is min value & other side is max value. minimum side i'm giving 10m/s velocity. Three module wattage respectively 150w,90w,60w.
Heat transfer coefficient is 10w/k.m.I'm new to analysis filed .what if ask boundary condition means what should i say.

 ghorrocks May 9, 2017 08:45

ANSYS Icepak does not have a forum for it - the fluent one may be more appropriate but I suspect not very useful.

But an overall comment: What heat transfer coefficient are you talking about? On the surface of the heat sink, or of the whole heat sink assembly?

 vigneshz259 May 9, 2017 11:46

ansys icepak boundary condition

For whole assembly. and also please explain to me what is convergence criteria.and difference between steady state thermal analysis & transient analysi.

 ghorrocks May 9, 2017 19:25

This is basic CFD modelling stuff - you need to do the tutorial examples and read the documentation to understand the basics. I am not going to rewrite a textbook in a forum post to explain basic concepts like that (sorry).

 guohanqing July 23, 2017 03:20

Hello,
When I was simulating a propeller in CFX, I used both steady and transient method, however the lift in transient is 10% higher than in steady method. I don't know why that great differences happened. Can anyone help explain that. The physical timescale in steady method is T*1/180。the time step in transient calculation is also T*1/180.

 ghorrocks July 23, 2017 04:20

Inaccurate simulation results can be caused by many things. Have a look in the FAQ page for the Ansys wiki on fd-online.

 All times are GMT -4. The time now is 06:12.