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

CFX varying response to mesh types

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

Like Tree4Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 6, 2024, 07:07
Default
  #21
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Dear Glenn, thanks for your kind response!


I have tried everything - opening type B.C., placing the outlet downstream up to 200D (D=pipe diameter), changing solver schemes, etc.


I can guarantee about the Physics and modeling that it is correct! Because for the same conditions, I have obtained good solutions. And with OPENFOAM, I have obtained very good results for a very coarse mesh with only 165000 Hexa-elements!! I checked mesh refinement also in OPENFOAM. It worked out pretty nice!


So far I observed that the solutions do not go further after the warning "wall placed at exit...." Moreover, CFX gives varied error messages - FINMES, Exit code 1, and sometimes with no error but code abruptly achieves convergence criteria, and exits. This inconsistent behavior from the CFX solver is what puts me in more doubt.


No clues so far....
pkgupta is offline   Reply With Quote

Old   April 7, 2024, 07:33
Default
  #22
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
I could find some correlation between the near-wall grid and the particle size. Originally I was trying to simulate two-particles slurry, of particles sizes 125 and 440 microns. And no matter what refinement I used, the solver always detected "wall at the outlet..." possibly due to some re-circulation. So far I was trying with Steady state solver.


Today, I systematically tried to break down the problem and started from simpler models. Soon, I found that whenever my particle size exceeds near-wall grid size, the solver behaved as pointed above.


Then, I started with transient solver, with mesh size now consisting 394095 hexa elements only. Firstly I simulated with single particle of 440 micron. It was working fine and converging. Of course I had to use very low time step size. Increasing the time step size again caused warning "wall placed at outlet...".


Next, I included another particle of 125 micron to the 440 micron slurry. And currently the simulations are going on nicely!


At this juncture, I would like to have your expert opinion on the following:
1. Since transient simulations shall take a very long time for one simulation, can I run the same set up with STEADY state but using very low time scale? Will that work?


2. Since it is my first time using TRANSIENT solver, I am not very well informed about how to set the total time for converged solution? For e.g. my pipe length is 8 m and slurry flow is at mean flow of 1 m/s. Does it mean I have to run the simulations for 8/1 = 8 s? Can I not obtain good solution, for say, t = 1 s, when my time step = 0.001 s?


3. As I browsed various sites about these details, I found Courant number a major player in Transient runs. So, I am ensuring to keep my Max. Courant no. less than 0.75.


Sir, if you would like to give some more insights, it would be very helpful. Because I am having limited computational resources and time. So, please tell me the best way out to get TRANSIENT runs on a machine with Intel(R) Core(TM) i7-9700F CPU @ 3.00GHz 3.00 GHz with 64 GB RAM DDR4.


Thanks in advance!
pkgupta is offline   Reply With Quote

Old   April 7, 2024, 18:59
Default
  #23
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,732
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
It would be good if you showed some images of the recirculation at the outlet.

Yes, you can just change a steady state simulation to transient. I would not recommend using Courant number to define the time step size, I would use adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the max and min time step size are wide enough that it never hits them.

The total time you have to run for varies on what you are modelling. As you are trying to get the steady response, or at least see what the flow settles down to, then I would run it for a very long time (hours of flow time) and put the key output parameter to a monitor point. Then run it and watch the monitor point as it progresses. When you have run it long enough that you have what you need then you can stop the run manually.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 10, 2024, 10:28
Default
  #24
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
To my utter surprise, even the transient simulations failed to converge before even reaching 1 second time!



The same happened with Steady state solver but with physical time of 0.001 sec. In both cases, the solver EXITs without without any WARNING or ERROR, but simply showing that All residuals reached the convergence criteria of 1e-4.


Now, this is beyond my comprehension!
pkgupta is offline   Reply With Quote

Old   April 10, 2024, 14:56
Default
  #25
Senior Member
 
Join Date: Jun 2009
Posts: 1,816
Rep Power: 32
Opaque will become famous soon enough
Quote:
Originally Posted by pkgupta View Post
To my utter surprise, even the transient simulations failed to converge before even reaching 1 second time!



The same happened with Steady state solver but with physical time of 0.001 sec. In both cases, the solver EXITs without without any WARNING or ERROR, but simply showing that All residuals reached the convergence criteria of 1e-4.


Now, this is beyond my comprehension!
The Ansys CFX Solver is not that quiet. You must have missed something in the diagnostics.

Please check the output file for the residual diagnostics per iteration. I would not be surprised you got an "F" in some equations.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 10, 2024, 22:58
Default
  #26
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Yes, you are on dot Prof. Glenn!


I did notice 'F' in most of the residuals at the beginning of the iterations. IN fact, it was there in the very first iteration, but thereafter it vanished.
Here is the part of it at first timestep:
+--------------------------------------------------------------------+
| Writing transient file 0_full.trn |
| Name : Transient Results 1 |
| Type : Standard |
| Option : Timestep Interval |
+--------------------------------------------------------------------+


================================================== ====================
| Timestepping Information |
----------------------------------------------------------------------
| Timestep | RMS Courant Number | Max Courant Number |
+----------------------+----------------------+----------------------+
| 2.0000E-03 | 0.15 | 0.29 |
----------------------------------------------------------------------

================================================== ====================
TIME STEP = 1 SIMULATION TIME = 2.0000E-03 CPU SECONDS = 6.793E+01
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 6.793E+01
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-water | 0.00 | 9.2E-12 | 4.6E-10 | 5.4E+04 F |
| V-Mom-water | 0.00 | 8.2E-12 | 4.4E-10 | 6.3E+04 F |
| W-Mom-water | 0.00 | 3.6E-03 | 1.6E-02 | 4.4E-05 OK|
| U-Mom-d440 | 0.00 | 1.1E-12 | 5.3E-11 | 5.4E+04 F |
| V-Mom-d440 | 0.00 | 1.7E-03 | 1.7E-03 | 1.1E-05 OK|
| W-Mom-d440 | 0.00 | 4.1E-04 | 1.8E-03 | 4.4E-05 OK|
| U-Mom-d125 | 0.00 | 1.3E-12 | 6.4E-11 | 5.5E+04 F |
| V-Mom-d125 | 0.00 | 2.1E-03 | 2.1E-03 | 1.1E-05 OK|
| W-Mom-d125 | 0.00 | 5.0E-04 | 2.2E-03 | 4.4E-05 OK|
| Mass-water | 0.00 | 4.5E-10 | 1.8E-08 | 9.5E+02 F |
| Mass-d440 | 0.00 | 7.2E-10 | 2.9E-08 | 4.6E+02 F |
| Mass-d125 | 0.00 | 5.4E-10 | 2.2E-08 | 43.1 7.2E+02 F |
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 0.00 | 1.1E-01 | 3.6E-01 | 5.8 5.7E-09 OK|
| E-Diss.K-Bulk | 0.00 | 2.0E-01 | 7.8E-01 | 12.5 1.7E-14 OK|
+----------------------+------+---------+---------+------------------+



And then at the time step = 125, here again it showed before Exiting:


----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 2 CPU SECONDS = 7.897E+04
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-water | 0.00 | 1.1E-09 | 2.8E-07 | 2.3E+02 F |
| V-Mom-water | 0.00 | 1.7E-09 | 1.8E-07 | 2.3E+02 F |
| W-Mom-water | 0.00 | 1.4E-08 | 6.2E-06 | 3.1E+00 F |
| U-Mom-d440 | 0.01 | 9.6E-08 | 5.5E-05 | 5.3E-02 ok|
| V-Mom-d440 | 0.04 | 1.2E-06 | 5.4E-04 | 2.0E-02 ok|
| W-Mom-d440 | 0.02 | 4.7E-07 | 1.2E-04 | 6.6E-02 ok|
| U-Mom-d125 | 0.00 | 1.8E-10 | 1.2E-08 | 6.6E+02 F |
| V-Mom-d125 | 0.00 | 3.9E-10 | 2.3E-08 | 3.0E+02 F |
| W-Mom-d125 | 0.00 | 7.2E-10 | 2.2E-07 | 3.5E+01 F |
| Mass-water | 0.00 | 6.1E-13 | 2.0E-10 | 7.6E+02 F |
| Mass-d440 | 0.00 | 1.7E-08 | 1.0E-05 | 9.2E+01 F |
| Mass-d125 | 0.00 | 5.4E-13 | 1.6E-10 | 43.2 4.9E+02 F |
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 0.58 | 1.9E-03 | 6.3E-01 | 5.7 1.6E-02 OK|
| E-Diss.K-Bulk | 2.11 | 7.8E-03 | 1.0E+00 | 12.4 7.9E-04 OK|
+----------------------+------+---------+---------+------------------+


================================================== ====================
| Adaptive Timestepping Information |
----------------------------------------------------------------------
| Direction | Ratio | Last Value | Next Value | RMS Co | Max Co |
+----------------+-------+------------+------------+--------+--------+
| Unchanged | 1.000 | 1.6000E-03 | 1.6000E-03 | 21.31 | 999.99 |
+----------------+-------+------------+------------+--------+--------+

================================================== ====================
TIME STEP = 125 SIMULATION TIME = 2.0040E-01 CPU SECONDS = 7.932E+04
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 7.932E+04
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-water | 0.00 | 2.1E-11 | 5.5E-09 | 1.5E+05 F |
| V-Mom-water | 0.00 | 2.5E-11 | 3.4E-09 | 1.3E+05 F |
| W-Mom-water | 0.00 | 4.9E-10 | 2.1E-07 | 3.7E+02 F |
| U-Mom-d440 | 0.00 | 6.6E-09 | 2.2E-06 | 8.1E+01 F |
| V-Mom-d440 | 0.00 | 1.1E-07 | 2.8E-05 | 6.6E+00 F |
| W-Mom-d440 | 0.00 | 9.5E-09 | 2.1E-06 | 3.6E-02 ok|
| U-Mom-d125 | 0.00 | 1.2E-11 | 3.6E-09 | 1.1E+02 F |
| V-Mom-d125 | 0.00 | 1.6E-11 | 3.8E-09 | 2.9E+03 F |
| W-Mom-d125 | 0.00 | 8.4E-10 | 3.2E-07 | 1.9E+02 F |
| Mass-water | 0.00 | 5.5E-17 | 1.7E-14 | 4.3E+06 F |
| Mass-d440 | 0.00 | 4.0E-08 | 1.7E-05 | 1.1E+06 F |
| Mass-d125 | 0.00 | 8.9E-14 | 5.3E-11 | 9.4 1.6E+06 F |
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+






How could this impact the solutions after 100+ iterations??


Can you guide me to how to decipher each and every info that is in the OUT File? Is there any good reference available?



I can understand most of it, which are straight-forward.
pkgupta is offline   Reply With Quote

Old   April 10, 2024, 23:13
Default
  #27
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,732
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
A few points:
1) I am not a professor
2) It was not my suggestion, it was Opaques. I do not know if he is a professor
3) The CFX documentation describes the contents of the output file. But in short, those "F" show the linear solver failed to converge, but it proceeded anyway. It is common to have an F or two in the first iteration, but they must settle down and reliably converge for your result to be converged. You have consistent F the whole way through so your run was always going to fail.

The Fs are sign of poor numerical stability. Things to look at are:
* Mesh quality
* Mesh quality (it is worth mentioning twice. Any improvements to mesh quality will make a huge difference. Even if the diagnostics say the quality is OK, do it anyway)
* Smaller time step (but don't go too small)
* double precision solver
* better initial conditions
* ramp complex physics in carefully
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 10, 2024, 23:48
Default
  #28
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Thank you Glenn for your kind clarifications!


And I am sorry I didn't notice it was Opaque answering, because so far only Glenn had been communicating!

Thanks Opaque!


I purposely addressed you as Professor! To me Professor means who professes a theory or philosophy due to his/her expertise. Your expertise made me address you as Professor!


Now, coming back to your inputs:
1. Mesh quality - I have been checking everytime the mesh quality metrics, such as, skewness, orthogonality, determinant 2x2x2, aspect ratio, angle, etc.However, I would be very thankful if you can give me some figures for these metrics which could be helpful to solve the complex physics I am trying here.


2. I tried with deltaT=0.001 s. Now I will go further down to 0.0005 s.
3. I have always been using Double precision only
4. So far, my initial conditions are the same as the inputs parameters at the domain INLET. Do you suggest me to set different initial conditions?
5. Ramp complex physics carefully - You mean that I shall first get good converged solution for single particle, and then to that solution add the second particle and see what happens?


Thanks once again!
pkgupta is offline   Reply With Quote

Old   April 11, 2024, 00:11
Default
  #29
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,732
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Please upload your output file. Do not use a third party site - just put it as an attachment on this forum.

Also please post an image of your mesh, with a detail of the near-wall mesh. Also show an image of a typical result for the flow.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 11, 2024, 03:22
Default
  #30
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Thanks Glenn!


I am attaching two output files:
1. Adaptive Transient case
2. Only Transient case - IN this case also, the first iteration showed "F" for many residuals


The PDF file shows the mesh, near-wall details, with the mesh metrics. Also sample results showing the Volume fractions of the two particles are shown.


Transient only Case.txt

Adaptive Transient Case.txt

Mesh Images.pdf



pkgupta is offline   Reply With Quote

Old   April 11, 2024, 06:22
Default
  #31
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,732
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Your transient simulation uses time steps of 1ms, but the adaptive time stepping never gets as small as 1ms, it is 1.6 to 2ms. So it looks like you should put a maximum time step of 1ms as that can cause divergence.

Also I note you are using coupled VF solver. Try the segregated one, sometimes that can help.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 11, 2024, 17:13
Default
  #32
Senior Member
 
Join Date: Jun 2009
Posts: 1,816
Rep Power: 32
Opaque will become famous soon enough
Quote:
Originally Posted by pkgupta View Post
I tried coarsening the mesh, but still the same error, "Wall placed at outlet...."


Then I refined my mesh from 661500 elements to 2396160 hexahedral elements. Yet the same error persists, after 3 iterations only!


Could you extract any useful info from the OUT file?


I am still not very convinced about mesh size? In one Journal paper published in 2009, the authors reported mesh of 385600 elements only, but used Transient simulations. And the paper has reported several cases on mono-size solid-liquid flow validations against experiments.
On that basis only I am wondering why CFX is unable to produce results even with the finer meshes than the reported one in 2009!


After today's run with 2396160 elements, it is clear that it is not the mesh problem. Something else is going on here which we are not able to point to.


Hope you would have some answers...
Can you list the model simplification you have used that led to a successful simulation?

Complex multiphase modeling is not a trivial task. Using the same geometry, can you model converge using only the dominant phase?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 17, 2024, 21:25
Default
  #33
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Your transient simulation uses time steps of 1ms, but the adaptive time stepping never gets as small as 1ms, it is 1.6 to 2ms. So it looks like you should put a maximum time step of 1ms as that can cause divergence.

Also I note you are using coupled VF solver. Try the segregated one, sometimes that can help.

I tried your suggestions. Initially, segregated solver worked well, but eventually it led to the same warning - "walls placed at outlet...."


With adaptive time-stepping also, eventually the iterations did not converge!


All the above was when I selected "Steady State solver".


Unfortunately, I cannot afford to run "transient" simulations due to computational limitations at my disposal.
pkgupta is offline   Reply With Quote

Old   April 17, 2024, 21:33
Default
  #34
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Can you list the model simplification you have used that led to a successful simulation?

Complex multiphase modeling is not a trivial task. Using the same geometry, can you model converge using only the dominant phase?

Hi, Opaque!


You can find the modeling details in thread #30 dated 12th April, 2024.


And I don't understand what you meant by "dominant phase?" If you referred to 440 micron particle in the two-particle slurry system, then "yes", it is the dominant phase. And YES, when I use only the mono-sized slurry, the solutions converge properly, for the same geometry.
pkgupta is offline   Reply With Quote

Old   April 17, 2024, 21:42
Default
  #35
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,732
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Have you had a look at the outlet boundary to see why there is backflow? Is it in the boundary layer adjacent to a wall? Or in the bulk flow? Or a vortex convected from upstream?

There is nothing special about adaptive time stepping, it just sets the time step. So if adaptive time stepping and your setting a time step gives different results it is because the time step size the two approaches are using give different results. It is not adaptive time stepping's fault, it is the time step it is giving which is the problem. But in this case you appear to be highly sensitive to time step size so you probably need to directly set the time step - so let's just stay with setting the time step size manually.

You need to do something to stop this continuous failure of the linear solver. That is what is leading to the divergence later on.
Opaque likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 18, 2024, 11:00
Default
  #36
New Member
 
Pawan K Garg
Join Date: Apr 2010
Location: India
Posts: 24
Rep Power: 16
pkgupta is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Have you had a look at the outlet boundary to see why there is backflow? Is it in the boundary layer adjacent to a wall? Or in the bulk flow? Or a vortex convected from upstream?

There is nothing special about adaptive time stepping, it just sets the time step. So if adaptive time stepping and your setting a time step gives different results it is because the time step size the two approaches are using give different results. It is not adaptive time stepping's fault, it is the time step it is giving which is the problem. But in this case you appear to be highly sensitive to time step size so you probably need to directly set the time step - so let's just stay with setting the time step size manually.

You need to do something to stop this continuous failure of the linear solver. That is what is leading to the divergence later on.

Dear Glenn! In most of your responses, I found that you have many times asked me to Check the outlet boundary flow for backflow etc. And I have been wondering how I can check this because my solutions are never reaching convergence criterion; and mostly solver exits without any results file.


Recently while going through your earlier posts (elsewhere on CFD-online), I noticed in CFX-Pre>Output control Tab> Results Tab, where several options are available. When I chose <Selected variables> I could find the following:
1. Output equations residuals
2. Output boundary flows
3. Output variable operators


Now, my question is whether I need to check <output boundary flows> option? And if yes, then which variable is of our interest to Check backflow?
pkgupta is offline   Reply With Quote

Old   April 18, 2024, 19:15
Default
  #37
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,732
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The key thing you should check is to load the flow into the CFD-Post so you can see exactly what the flow is doing. If your simulation does not complete and therefore there is no results file then you need to either manually save a backup file in Solver Manager while it is still running, or set it to automatically save a backup file before it crashes.

If you can see what the flow is doing it that will determine what you need to do to fix it.
Opaque likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
cfx, wall at outlet error

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
foam-extend-4.1 release hjasak OpenFOAM Announcements from Other Sources 19 July 16, 2021 05:02
[snappyHexMesh] non uniform mesh near the stl object vava10 OpenFOAM Meshing & Mesh Conversion 0 January 31, 2021 14:41
GeometricField -> mesh() Function Tobi OpenFOAM Programming & Development 10 November 19, 2020 11:33
[Gmsh] 2D Mesh Generation Tutorial for GMSH aeroslacker OpenFOAM Meshing & Mesh Conversion 12 January 19, 2012 03:52
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Meshing & Mesh Conversion 2 March 27, 2011 21:11


All times are GMT -4. The time now is 15:20.