Simulation Forums

Find Simulation answers, share expertise, and connect with your peers

Simulation CFD


advection Scheme

128 Views, 8 Replies
03/09/2018 5:03 PM

Hello, 

I want to put light on several aspect of advection scheme. 

When i do a simulation i generally proceed this way  (simulation implies most of the time a centrifugal fan) : 

 

  1. Modelise my real fan with a cylinder and use centrifugal blower material 
    1. For the first simulation I generally go with a : 
      1. autosize meshing
      2. auto convergence assessement : loose
      3. advection scheme #1 (montone streamline Upwind)
      4. k-epsilon turbulence model  with no IWF
    2. For the next simulation I generally want to know ''how many element i need to have a solution who become independent from meshing''. To achieve that i just put convergence assessement to (loose/default) and gradually increase the number of mesh. Since i'm confident that I reach this objective i switch to the advection scheme #5 (Modified Petrov-Galerkin) . I reproduce the same protocole from the previous step (#1)
  2. Modelise my real fan (blade, shaft ...) with RR and use advection scheme #5 (default setting for rotating region).
    1. Start with k-epsilon 
    2. Finish with k-omega (bench mark test)   

From what I read in autodesk blog, adv1 seems a scheme who's very robust and give you a general ideal of the simulation while adv5 is the most accurate. 

 

Regarding the fact that I use centrifugal blower, for my fisrt part of analysis can i choose smoothing else than adv1 ? 

for example adv 1 ''is diffusive for meshes not aligned with flow'' not sure what this sentence mean since my element has a triangular form. In some case can the adv#2 is more suitable ? 

 

Futhermore when i'm switching to k-omega turbulence model (with RR) I obtain totaly different pressure and velocity distribution and turbulent energy dissipation , TED.

My feeling said that the k-omega(adv5) model is more accurate than the k-epsilon (adv1).

Considering the fact that my ''first step simulation'' give me differente result that k-omega simulation what kind of information that I need to be aware of when i'm running ''the first step'' simulation : 

  • high gradient zone? 
  • general behavior ?
  • recirculation over BC ?
  • meshing dependence ? 
  • what information can i get from plot convergence ? 

 

Finally, I know the general line about turbulence model et adv scheme but this link keep me hungry of knowledge. Do you have something else ? 

 

Merci 
Frederic 

 

PS what should be a reasonable time step increment for centrifugal blow

 

 

 

 

 

 

Report Inappropriate Content
Message 1 of 8 ( Views: 128 )

Re: advection Scheme

03/12/2018 9:58 AM

Hi Fred,

 

ADV 5 is now the default advection scheme in CFD2018. It has gone through rigorous testing and has proven to give more accurate results than ADV1 in most cases and is just as robust. I would therefore simply start with ADV5 and save yourself some time.

 

for example adv 1 ''is diffusive for meshes not aligned with flow'' not sure what this sentence mean since my element has a triangular form.

 

Very good point. Maybe it means that ADV1 is only good with extruded meshes. I will ask around!

 

In some case can the adv2 is more suitable ? 

 

Definitely always use ADV5 rather than ADV2. ADV2 is older version of ADV5.

 

Here is the updated info on advection schemes. And for info on turbulence models have a look at this page and also this webinar

 

If you simply switch between the k-e and k-o models you will get very different results as the k-o has different meshing requirements. For k-o you should aim for Y+ less than 2 (the webinar will explain), this will require tight refinement near the wall using many wall layers and a high gradation.

 

Does that help?

 

All the best,

David


David Short
Technical Support Specialist, Simulation

Report Inappropriate Content
Message 2 of 8 ( Views: 112 )

Re: advection Scheme

03/15/2018 3:07 PM

Hello David, 

thank for your answer, few question remain. 

 

  1.  From your perspective which turbulence model is more approrpriate for this specific case and why ?
    1. From my point of view i will say k-omega because since the exhaust is narrow, edge effect has to be considered to simulate the flow correctly. 
  2. Since I reach mesh independency with an autosizing mesh and an uniform meshing , is there any difference between those two proceedure (accuracy, result and time calculation perspective ) ? 
  3. For the exact same setup,  why there has a difference between transicient  and steady state mode solution ?
    1. If you look on the two last graph (k-omega model) you see considerable pressure rise over the whole model. However, other parameter seems to be coherent with the steady state solution model.
    2. Finally, how you choose the appropriate time step and how the time step can affect the accuracy of the simulation?
      1. from  what I read in the forum you should converge after 500 - 600  iterations. 
      2. I have the same question for the RR with a six blade fan. (0.002778sec); are we taking advantage to use smaller time step for RR (3deg for time step)  

In the word document i only display static pressure, velocity vary too much from a model to another. Don't hesitate if something remain unclear in the document. 

 

coarse sim_support.cfz :     k-epsilon [ Sc1 - copy(1)  to  Sc1 - copy(6) ] 

First Attempt_support.cfz : k-omega [ Sc1 - copy(7)  to  Sc1 - copy(8) ]

Report Inappropriate Content
Message 3 of 8 ( Views: 103 )

Re: advection Scheme

03/19/2018 8:58 AM

Hi Fred,

 

Sorry for the late reply but i thought maybe going at it with a fresh Monday mind would be better! Thanks a lot for taking the time to report your findings.

 

1. From your perspective which turbulence model is more appropriate for this specific case and why ?

 

I think both could work when using the blower material however different mesh characteristics will be required. 

 

When using an RR I would just use SST K-omega as capturing the flow separation off the blades is of key importance. K-epsilon struggles in this area!

 

2. Since I reach mesh independency with an autosizing mesh and an uniform meshing , is there any difference between those two procedure (accuracy, result and time calculation perspective ) ? 

 

If you are sure that you have mesh independent results then go with which ever approach is less mesh intensive i.e. lower element count as this will reduce run time. By definition If the solution is mesh independent then you cannot have improvements in accuracy using an alternative mesh as the results should be the same. 

 

3. For the exact same setup,  why there has a difference between transient and steady state mode solution?

 

You can think of a steady state solution as being similar to an infinite transient solution (one that has been run for a long time until it is fully converged) for a problem where boundary conditions remain constant. A transient solution would then have to be completely converged to allow comparison with the steady state solution. This takes a long time as at each time step a new steady state problem is posed to the solver, it then uses inner iterations (similar to iterations in a steady state simulation) to find the converged solution at that time step. Far fewer inner iterations are needed than normal iterations in a steady state solution due to stability improvements in the equations introduced by temperol discretization (time dependent terms) and also because the solution from the previous time step is used as the initial condition for the next, meaning that not much variation in flow and HT needs to be computed. 

 

To accurately model transient behaviour in a simulation you must select a time step with respect to the time scale of the flow. For example when the flow is complex you need a very small time step to minimize the change in flow between steps. Using a larger time step would create a 'chunky' solution and detail would be lost between the steps, big jumps in solution between time steps will likely cause the solver to crash. Therefore start with a fairly large time step of say 0.5 seconds and then compare with one of 0.1 seconds, checking for solver stability (i.e. not diverging and crashing) and realistic visualisation of flow behaviour (not chunky jumps).

 

Does that answer your questions?

 

All the best,

Dave

 


David Short
Technical Support Specialist, Simulation

Report Inappropriate Content
Message 4 of 8 ( Views: 95 )

Re: advection Scheme

03/19/2018 7:10 PM

Hello David, 

Thx for you exhaustive answers. It's very clear. 
Last one before i close the subject : 

Can I run steady state solution with a RR?
Danke

Fred


Report Inappropriate Content
Message 5 of 8 ( Views: 89 )

Re: advection Scheme

03/20/2018 8:34 AM

Hi Fred,

 

All motion analyses including rotating regions need to be run transiently because at each time step the solution matrix changes (due to the moving mesh) thus there is no single matrix that can be solved to give a steady state solution for the whole process. 

 

There is a flag called FrozenRotor which can simplify the RR analysis and allows for larger time steps. You could maybe try running that steady state but I am not sure if it works!

 

All the best,

David


David Short
Technical Support Specialist, Simulation

Report Inappropriate Content
Message 6 of 8 ( Views: 82 )

Re: advection Scheme

03/20/2018 2:02 PM

Thx Again David, 

I'm looking forward to share this knowledge to others through this forum. 
Have a nice week.

Fred


Report Inappropriate Content
Message 7 of 8 ( Views: 73 )

Re: advection Scheme

03/20/2018 2:06 PM

Always a pleasure Fred!

 

Have a good one,

David


David Short
Technical Support Specialist, Simulation

Report Inappropriate Content
Message 8 of 8 ( Views: 70 )