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

Convergence issue- ANSYS CFX - Ceiling Fan CFD analysis

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

Like Tree8Likes
  • 1 Post By Opaque
  • 1 Post By Opaque
  • 2 Post By Gert-Jan
  • 1 Post By Gert-Jan
  • 1 Post By Gert-Jan
  • 1 Post By Gert-Jan
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 7, 2020, 06:42
Default Convergence issue- ANSYS CFX - Ceiling Fan CFD analysis
  #1
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Hi I am using ANSYS CFX to solve CFD analysis of Household Ceiling fan. My intention is to find the Air delivery of ceiling fan by replicate the actual test scenario. The test is conducted by placing the the ceiling fan in a standard test chamber at a height of 3 meters from the floor and measure the velocity values at a plane 1.5 m from the plane and along 4 diagonal axes (details of test chamber and measuring points are included).
I am conducting steady state analysis in ANSYS CFX with a time scale of 1/omega and for meshing I am using ICEM CFD. My problem is not getting proper convergence. The residual target set was E-04 but not achieving this for 2000 iterations. The monitoring points are also not steady.
I need to conduct a detailed Grid independence test but my doubt is how to conduct this. I am doing the mesh in ICEM CFD with a global size of 100 mm and different sizing at wall, fan surface and also created a cone like shape to refine the mesh at my flow field (Images included- the cone like structure added only for refine the mesh at flow field)). Here while doing grid test which mesh I need to change whether the global element size or Local element size at my flow field. Also How I terminate my analysis while doing the grid test as my problem not giving termination based on residual target. So how I decide the total number of iterations.

Please help me

1. Thing I need to look for getting convergence
2. How to conduct Grid test whether to change global size or change local size
3. How to terminate the simulation while doing grid test
4. Suggestion to improve meshing strategy

Residuals.JPG

Monitoring point.JPG

10.jpg

Test chamber.JPG

velocity measure.JPG

Last edited by Deepaksha; July 7, 2020 at 10:47. Reason: Spelling mistake
Deepaksha is offline   Reply With Quote

Old   July 8, 2020, 12:04
Default
  #2
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Hi Somebody please help me
Deepaksha is offline   Reply With Quote

Old   July 8, 2020, 12:23
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,365
Rep Power: 25
Opaque will become famous soon enough
I am confused by your intent to avoid the residual convergence.

You intend to solve a mathematical problem --> solve the flow equations

The metric provided to verify the problem has been solved IS the residual norm, correct? The theoretical value is supposed to 0, the software allows you to relax it to say 1E-04 (empirical value)

You intend to analyze an intermediate data point that does not satisfy the criteria of "has been solved", and plan to consider such a solution the solution to your problem. Did I understand your request correctly?

What is the point of the calculation then?
Deepaksha likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   July 8, 2020, 13:23
Default
  #4
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Thank you very much for your response. I am looking to get a converged solution. I have set a residual target of 1E-04 which is said to be a good accuracy but as you can see in the image the residuals not reaching this value. I have allowed the solution to run till 2000 iteration but it not seems to meet the target. So I created monitoring points for velocity which is my area of interest and it also showing large variation.

What I need to look for getting a converged solution (I thought it might be problem with meshing that is why I raised questions regarding Grid test)

More details of my problem

Model creation
Assembly of Celling Fan placed in Standard AD chamber as per IS 374-1979. Then Extract Fluid volume from the assembly and split the Fluid volume into two part in such a way that Fan including near by volume in a cylindrical shape is consider as Rotor and the remaining portion consider as stationary domain. The cylindrical volume cut by taking an offset dimension of 25 mm from Fan model extremities

3 doaminns "Rotor" (RPM -300), Stator & Cone (added for refinement)
MRF methode

Frozen rotor interface b/w Rotor and stator
General connection between staionary domains

Mesh- Tetra hedral mesh created with ICEM CFD
No of Nodes 1.6 Million

Steady state analysis
Fluid Domain
Material - air at 25c
reference pressure 1 atm
SST turbulence model

Wall boundary condition for Fan surface and all the walls
No inlet or outlet
Only domain rotation is specified no other parameters set

Solver control
Advection scheme - High resolution
Turbulance numerics - High resolution
Physical time scale - 1/omega

Kindly give guidance to get a converged solution I am a beginner it will be very helpful If you can guide which are the areas I need to look for a converged solution.
How I need to approach the problem. If any more clarification or details of problem is required , i can provide
Deepaksha is offline   Reply With Quote

Old   July 8, 2020, 14:03
Default
  #5
Senior Member
 
Join Date: Jun 2009
Posts: 1,365
Rep Power: 25
Opaque will become famous soon enough
Just another minor clarification: residuals are not related/correlated with accuracy in any way or form either. Residuals are a measure of convergence. You can get a well-converged solution that is also rubbish; therefore, no connection.

Residuals --> how well we solved the set of equations

Discretization Error --> difference between the current solution, and the exact solution (discretization parameters independent)

Model error --> difference between what the real solution should be and what the equations can represent.

There is a lot of confusion and misusage of those words in the CFD community. Used in the wrong context will lead to wrong conclusions.

Now, how to help with the convergence of a given problem. You need to understand where the residuals remain large; therefore, you must visualize and determine where the residual distribution is large. In ANSYS CFX, you can also output the residuals as a solution field and create plots in CFD-Post. Locate where the maximum residual is and try to correlate it with the flow conditions, mesh quality, etc. You must be able to tell if that region is of any significance and the residuals are just noise or not before dismissing them
Deepaksha likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Last edited by Opaque; July 8, 2020 at 14:09. Reason: Complete message
Opaque is offline   Reply With Quote

Old   July 8, 2020, 17:21
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20
Gert-Jan will become famous soon enough
Poor convergence can also occur if you solution is transient. Meaning: You told CFX to look for a steady state solution, but maybe there is none. If so, then CFX won't find it and won't converge. Given the fluctuating velocities, this might be the case. For now I would increase or decrease the time step with a factor 10. And see if this helps CFX to find a steady state solution. if it does not help, do a transient case using Frozen rotor. This might converge to a steady state.

If this does not help, then simplify your system to an axisymmetryc one. Take only 1/3 of your geometry. It is wise to use that anyway in a grid study. This means that you ignore the influence of the rectangular box around it. This will help convergence, provided your mesh is good enough.

After the grid sudy, extend again to full 3D and perform a transient calculation using Rotor-stator-interaction.
Opaque and Deepaksha like this.
Gert-Jan is online now   Reply With Quote

Old   July 9, 2020, 02:41
Default
  #7
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Just another minor clarification: residuals are not related/correlated with accuracy in any way or form either. Residuals are a measure of convergence. You can get a well-converged solution that is also rubbish; therefore, no connection.

Residuals --> how well we solved the set of equations

Discretization Error --> difference between the current solution, and the exact solution (discretization parameters independent)

Model error --> difference between what the real solution should be and what the equations can represent.

There is a lot of confusion and misusage of those words in the CFD community. Used in the wrong context will lead to wrong conclusions.

Now, how to help with the convergence of a given problem. You need to understand where the residuals remain large; therefore, you must visualize and determine where the residual distribution is large. In ANSYS CFX, you can also output the residuals as a solution field and create plots in CFD-Post. Locate where the maximum residual is and try to correlate it with the flow conditions, mesh quality, etc. You must be able to tell if that region is of any significance and the residuals are just noise or not before dismissing them

How can I plot the residuals in CFD post to locate where the maximum residual. can you please put some light on this
Deepaksha is offline   Reply With Quote

Old   July 9, 2020, 02:45
Default
  #8
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
Poor convergence can also occur if you solution is transient. Meaning: You told CFX to look for a steady state solution, but maybe there is none. If so, then CFX won't find it and won't converge. Given the fluctuating velocities, this might be the case. For now I would increase or decrease the time step with a factor 10. And see if this helps CFX to find a steady state solution. if it does not help, do a transient case using Frozen rotor. This might converge to a steady state.

If this does not help, then simplify your system to an axisymmetryc one. Take only 1/3 of your geometry. It is wise to use that anyway in a grid study. This means that you ignore the influence of the rectangular box around it. This will help convergence, provided your mesh is good enough.

After the grid sudy, extend again to full 3D and perform a transient calculation using Rotor-stator-interaction.
Thanks for the response. Usually for transient state analysis we are using "transient rotor stator interface, what will be the difference while using a Frozen rotor interface for transient analysis
Deepaksha is offline   Reply With Quote

Old   July 9, 2020, 03:10
Default
  #9
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20
Gert-Jan will become famous soon enough
In Pre > Output control > Results, you can teel CFX to add the residual values to the results file.
Gert-Jan is online now   Reply With Quote

Old   July 9, 2020, 03:29
Default
  #10
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20
Gert-Jan will become famous soon enough
When running steady state, you are using false timesteps. In a transient case you use real timesteps. Not sure if it will help, but you can give it a try.

BUT: you have 3 impeller blades and your environment has 4 corners. This means that your flow will be transient. Period. No software package will ever find a steady state. Steady State calculations are a waste of time.

Therefore, if you want to perform a grid study, then: What question are you trying so answer using CFD?
1) If you need to solve the flow around the fan and the ceiling in detail, better simplify your geometry to an axisymmetric one, ignoring the rectangular environment. This environment will lead to transient effects, screwing up your steady state solution around your impeller. Therefore: simplify.
2) If you need to solve the interaction with the environment, then you're in trouble if you want to do a grid study. As mentioned previously, you need to do real transient rotor-stator-interactions, perform time averaged results (number of revolutions to average is a parameter to investigate) and compare these in the grid study.

I hope you have a large computer.
Deepaksha likes this.
Gert-Jan is online now   Reply With Quote

Old   July 9, 2020, 05:38
Default
  #11
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
When running steady state, you are using false timesteps. In a transient case you use real timesteps. Not sure if it will help, but you can give it a try.

BUT: you have 3 impeller blades and your environment has 4 corners. This means that your flow will be transient. Period. No software package will ever find a steady state. Steady State calculations are a waste of time.

Therefore, if you want to perform a grid study, then: What question are you trying so answer using CFD?
1) If you need to solve the flow around the fan and the ceiling in detail, better simplify your geometry to an axisymmetric one, ignoring the rectangular environment. This environment will lead to transient effects, screwing up your steady state solution around your impeller. Therefore: simplify.
2) If you need to solve the interaction with the environment, then you're in trouble if you want to do a grid study. As mentioned previously, you need to do real transient rotor-stator-interactions, perform time averaged results (number of revolutions to average is a parameter to investigate) and compare these in the grid study.

I hope you have a large computer.

Thank you for the response. As you said if i am simplifying the geometry to symmetrical shape say a cylinder there by avoid the rectangular shape then how I will set the boundary condition Top portion as inlet and bottom potrtion as outlet or both side as Opening ?
Deepaksha is offline   Reply With Quote

Old   July 9, 2020, 05:42
Default
  #12
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20
Gert-Jan will become famous soon enough
Set them is opening, but put them far away.
Deepaksha likes this.
Gert-Jan is online now   Reply With Quote

Old   July 9, 2020, 07:14
Default
  #13
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
In Pre > Output control > Results, you can teel CFX to add the residual values to the results file.
How can I visualize the same in CFD post
Deepaksha is offline   Reply With Quote

Old   July 9, 2020, 09:28
Default
  #14
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20
Gert-Jan will become famous soon enough
I don't understand your question.

What I proposed is to tell CFX that it should save the residuals in the results file after finishing the run. You tell this to CFX this in Pre, as suggested above.
Then run the case, and open the results file in Post. And you will find the residuals as variables to plot. Capice?
Gert-Jan is online now   Reply With Quote

Old   July 9, 2020, 10:57
Default
  #15
New Member
 
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5
Deepaksha is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
I don't understand your question.

What I proposed is to tell CFX that it should save the residuals in the results file after finishing the run. You tell this to CFX this in Pre, as suggested above.
Then run the case, and open the results file in Post. And you will find the residuals as variables to plot. Capice?
I got that point of saving the residuals in the result file. I was asking how can I locate the max residual point in my model. In which form I need to plot the variable. Whether I need to insert a point ? or any other kind of location parameter.

Very thankful to your every response and valuable time. It is very helpful to beginners like me.
Deepaksha is offline   Reply With Quote

Old   July 9, 2020, 11:30
Default
  #16
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20
Gert-Jan will become famous soon enough
Don't you have a supervisor who you can ask?

Just make an isosurface for a residual value of interest. The higher, the smaller the isosurface. It could be hard to see. Then turn of the Wireframe, choose Fit view and turn Wireframe back on. Then you can see where the highest residual is.
Deepaksha likes this.
Gert-Jan is online now   Reply With Quote

Old   July 9, 2020, 15:36
Default
  #17
Senior Member
 
Join Date: Jun 2009
Posts: 1,365
Rep Power: 25
Opaque will become famous soon enough
With Gert-Jan's approach you can visualize region at a given value, or above/below a given value which gives a great view of how the residuals are spread over the domain.

But, if you want to know exactly where a specific maximum/minimun residual is located, insert a point, select the residual of interest and select Maximum. You should get a cross-hair at the different locations where such value exists.

Hope either methodology allows you to get a better understanding of where the solution is stuck
Deepaksha likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Reply

Tags
convergence, icem cfd meshing, mesh and grid

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
ANSYS CFX 14 on UBUNTU 12.04 64bit: PARALLEL ISSUE david.pasquale CFX 6 August 9, 2018 15:05
CFD Salary CFD Main CFD Forum 17 January 3, 2017 17:09
Can you help me with a problem in ansys static structural solver? sourabh.porwal Structural Mechanics 0 March 27, 2016 17:07
cfd analysis of fan jyotinkateshia FLUENT 8 January 24, 2014 12:15
Pump Cavitation Analysis in ANSYS CFX techCAE CFX 6 July 3, 2013 06:37


All times are GMT -4. The time now is 14:09.