CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Steady state converges but transient does not

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 18, 2020, 01:26
Default Steady state converges but transient does not
  #1
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Greetings,

I am working on the simulation of flow inside a centrifugal fan, the first stage of design validation was a steady-state simulation where everything ran smoothly.

For the next stage of my design, I must run a transient simulation (this is because I need to do acoustic analysis), however, despite a lot of attempts the solution diverges after a couple iterations, can't even complete one time-step. (I always get the floating point exception)

Has anyone faced a similar issue? Please find details below

Steady-state info
  1. Pressure Inlet
  2. Mass flow outlet
  3. k-w SST turbulence model
  4. rotational speed = 25,000 RPM
  5. Interface= frozen rotor
  6. Monitor was placed to check the convergence of the pressure rise across the fan
As stated everything good with steady state.

For transient simulation I started with the same B.C's and a time step of 6.67e-6 (aware that I should do sensitivity analysis on this later on), I also started with the DES turbulence model and after failing with that, I tried some computationally simpler ones without success.

I think that summarizes everything, I appreciate any guidance or tip.

Regards
nihil2718 is offline   Reply With Quote

Old   February 18, 2020, 08:20
Default A few points
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
Is this in Fluent or CFX. Though valid, frozen rotor is not a terminology we use in Fluent. Is it full model or periodic model?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 18, 2020, 08:33
Default Steady state converges but transient does not
  #3
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
Is this in Fluent or CFX. Though valid, frozen rotor is not a terminology we use in Fluent. Is it full model or periodic model?
Hello Vinerm, thanks for your reply. I am doing it in Fluent (so MRF it is) and it is a full model. I already did both steady and transient in CFX without any problem.
nihil2718 is offline   Reply With Quote

Old   February 18, 2020, 14:47
Default MRF and Mesh Motion
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
Could you share a snapshot of two settings in your case?

1. Cell Zone Conditions
2. Boundary condition for the interface (is it interior between rotating and stationary frame or an interface?)
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 18, 2020, 20:50
Default Steady state converges but transient does not
  #5
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Please find below the information,

1. Cell zones
There are two cell zones, impeller and casing, both fluid. For the transient simulation impeller zone has mesh motion activated.

2. Boundary conditions at interface

What I did here was just create and name the interface after loading the mesh in Fluent (the name of the interface is "this is it").
Attached Images
File Type: jpg cell zone.jpg (95.5 KB, 40 views)
File Type: jpg interface.jpg (65.1 KB, 34 views)
File Type: png interface2.png (73.6 KB, 27 views)
nihil2718 is offline   Reply With Quote

Old   February 19, 2020, 04:00
Default Conditions
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
That's good but I apologize for not being more descriptive. I need to look at the conditions you have for cell zone. So, you need to open cell zone conditions and not just the tree, the option where frame motion and mesh motion are applied.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 19, 2020, 04:49
Default Steady state converges but transient does not
  #7
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Not at all!, my apologies for missing that info. Please find the cell conditions attached.

Let me know any other info you want to check.

Thanks
Attached Images
File Type: jpg conditions.jpg (125.6 KB, 45 views)
nihil2718 is offline   Reply With Quote

Old   February 19, 2020, 05:05
Default Two points
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
Now, check two things.

1. Is the axis of the rotor really aligned with z-axis as given in the mesh motion setting? Since axis is not visible in the images, I can't say that. Also check if the axis passes through the origin. For MRF, these settings, if improper, will let the case run but lead to wrong results. For moving mesh, case will not run.

2. Type of interface. What kind of settings have you used when defining the interface? Could you share that image as well? Before sharing, you may look at the first point. If that is the issue, you do not need to share the image and your case should run fine after defining proper reference point and rotation axis.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 19, 2020, 06:58
Default Steady state converges but transient does not
  #9
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
1. Yup, double checked, 100% sure it is aligned with the z-axis

2. I attached the image when I defined the interface

Regards
Attached Images
File Type: jpg interface creation.jpg (98.8 KB, 31 views)
nihil2718 is offline   Reply With Quote

Old   February 19, 2020, 07:03
Default Zone Motion
  #10
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
It seems to be all good. Last thing to check is if the motion is correct. With mesh motion setup, Fluent allows you to move the zone without any simulation. This is doable from Run Simulation panel (also from Dynamic Mesh panel). Display the mesh of the rotor alone and then use Display Zone Motion to observe the rotor move. Check if it moves properly or not. If it does, then the case would require a thorough check. If it does not show the expected motion, then you would be able to find the reason. Ensure to save your case file before displaying the zone motion because Fluent does not bring it back to the same position once the zone has moved.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 20, 2020, 03:50
Default
  #11
Senior Member
 
Andrea
Join Date: Feb 2012
Location: Leeds, UK
Posts: 179
Rep Power: 16
Andrea1984 is on a distinguished road
Hi Jorge,

this puzzles me since usually unsteady algorithms are more stable than steady ones.

What p-v coupling algorithm are you using? What is the Courant number value associated with your time-step? And what discretisation schemes are you using in time and space?

Also, are you using a psuedo-transient formulation for your "steady-state" run?

Cheers,
Andrea
Andrea1984 is offline   Reply With Quote

Old   February 20, 2020, 07:14
Default Steady state converges but transient does not
  #12
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
I checked the mesh motion and it seems fine the impeller rotates properly.

I keep thinking what can be the source of the problem but can't come with anything significant. If you come across any other parameter/setting I could check, let me know. Thanks again for the interest!

Regards
nihil2718 is offline   Reply With Quote

Old   February 20, 2020, 07:55
Default
  #13
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Quote:
Originally Posted by Andrea1984 View Post
Hi Jorge,

this puzzles me since usually unsteady algorithms are more stable than steady ones.

What p-v coupling algorithm are you using? What is the Courant number value associated with your time-step? And what discretisation schemes are you using in time and space?

Also, are you using a psuedo-transient formulation for your "steady-state" run?

Cheers,
Andrea
Hi Andrea, thanks for your message.

I attached and image with the info you requested for how I am trying to run the transient simulation. I am not quite sure what to answer in my selection of the time-step, I went for a relative short time-step (basically one time step for every degree the impeller rotates) as a starting point and was planning to do a sensitivity analysis on it later on.

How would you define the Courant number for this case?

For the steady-state I did use the pseudo-transient formulation with default settings, I used quite extensively to create the characteristic curve of the fan.

Regards
Attached Images
File Type: jpg solution methods.jpg (91.6 KB, 31 views)
nihil2718 is offline   Reply With Quote

Old   February 20, 2020, 07:55
Default Issue
  #14
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
If the impeller rotates as expected, then the only thing left is numerical setup. Since the time-step is already very small, problem could be with initialization or meshes at the interface. Since you already have MRF results, initialize using those and not from scratch. Secondly, check if meshes on both sides of the interface are similar to each other in size (possibly, you have already ensured it).
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 20, 2020, 09:35
Default
  #15
Senior Member
 
Andrea
Join Date: Feb 2012
Location: Leeds, UK
Posts: 179
Rep Power: 16
Andrea1984 is on a distinguished road
Hi Jorge,

I am not a Fluent user anymore but you should have a Convective Courant Number variable available to plot (if it is not, you should be able to create it using a custom field function). It is true that your time-step "sounds" small in absolute terms, still I would make sure that the maximum Courant number is below 1, especially when using PISO for pressure-velocity coupling. I would also suggest to test other pv-coupling algorithms less sensitive to the Courant number value such as SIMPLE or SIMPLEC.

Finally I would switch all the spatial and temporal discretisation schemes to first order until you fix your convergence problems. I am particular suspicious of the BCD for the convective term in the momentum equation. Why BCD and not 2nd order upwind (if you want to retain 2nd order accuracy)? After all, you are performing a (U)RANS simulation, BCD is more for LES and can lead to stability issues.

Andrea
Andrea1984 is offline   Reply With Quote

Old   February 23, 2020, 03:39
Default
  #16
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Quote:
Originally Posted by Andrea1984 View Post
Hi Jorge,

I am not a Fluent user anymore but you should have a Convective Courant Number variable available to plot (if it is not, you should be able to create it using a custom field function). It is true that your time-step "sounds" small in absolute terms, still I would make sure that the maximum Courant number is below 1, especially when using PISO for pressure-velocity coupling. I would also suggest to test other pv-coupling algorithms less sensitive to the Courant number value such as SIMPLE or SIMPLEC.

Finally I would switch all the spatial and temporal discretisation schemes to first order until you fix your convergence problems. I am particular suspicious of the BCD for the convective term in the momentum equation. Why BCD and not 2nd order upwind (if you want to retain 2nd order accuracy)? After all, you are performing a (U)RANS simulation, BCD is more for LES and can lead to stability issues.

Andrea

Hi Andrea,

Well I was using that particular configuration of spatial and temporal discretization schemes because for my analysis I need DES turbulence model and those are the schemes recommended in the users guide.

I did a rough estimate of my model to see what the Courant Number should be and it turns out it should be on the order of 10^-7, so I run a simulation with the steady-state one as initial values and still got divergence(I follow your advice and decided to run everything with first order accuracy and just the k-w SST model for turbulence). I attached an image of the residuals and of my monitor.

Any ideas on what could be the problem?

Regards
Attached Images
File Type: jpg Transient_1.jpg (94.3 KB, 20 views)
File Type: jpg Transient_@.jpg (94.0 KB, 17 views)
nihil2718 is offline   Reply With Quote

Old   February 23, 2020, 03:44
Default
  #17
New Member
 
Jorge
Join Date: Dec 2019
Posts: 10
Rep Power: 6
nihil2718 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
If the impeller rotates as expected, then the only thing left is numerical setup. Since the time-step is already very small, problem could be with initialization or meshes at the interface. Since you already have MRF results, initialize using those and not from scratch. Secondly, check if meshes on both sides of the interface are similar to each other in size (possibly, you have already ensured it).
I took for granted that the size at the interfaces were similar, however I am not sure to tell whether it is appropriate or not, I attached the interface sides for each component and I appreciate your comments on it.

Regards
Attached Images
File Type: jpg interface-impeller.jpg (97.4 KB, 31 views)
File Type: jpg interface-volute.jpg (105.2 KB, 23 views)
nihil2718 is offline   Reply With Quote

Old   February 23, 2020, 06:18
Default Curvature
  #18
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
Looking at the front image won't help. You need to observe the elements in the plane of rotation. That will show edges of the mesh capturing the curvature, similar to an octagon circumscribing or inscribing a circle. Both boundaries should have enough elements along the curvature or else there will be one element going inside the other and that will cause trouble.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 25, 2020, 04:06
Default
  #19
Senior Member
 
Andrea
Join Date: Feb 2012
Location: Leeds, UK
Posts: 179
Rep Power: 16
Andrea1984 is on a distinguished road
Hi Jorge,

I can't think of any obvious reason for this behaviour. I thought about possible issues with your mesh at the interface but this should show in your steady-state calculation as well.

Have you tried SIMPLE instead of PISO (retaining first order discretisation for everything?).

Also, why are you using 1000 iterations per time step? Is this in conjunction with some residuals-based criterion? I tend not to use the latter for transient simulations. I usually adjust the number of iterations per time-step based on a drop of about 2 orders of magnitude is the residuals. Normally I start with a low time step (max Co ~ 0.1 or even lower if necessary) and high number of iterations per time step (around 100), and then gradually increase the former and decrease the latter until I reach a good compromise between convergence and runtime.

Andrea
Andrea1984 is offline   Reply With Quote

Reply

Tags
acoustics, centrifugal fan, divergence, transient

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Steady State Vs Transient answers Kushagra CFX 25 July 23, 2017 03:20
Transient & steady simulation DIVYA P SOMAN ANSYS 0 September 3, 2016 14:09
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56
Transient vs Steady State Adam CFX 1 April 12, 2007 11:34
About the difference between steady and unsteady problems Lisa Main CFD Forum 11 July 5, 2000 14:37


All times are GMT -4. The time now is 01:17.