
[Sponsors] 
Convergence issue ANSYS CFX  Ceiling Fan CFD analysis 

LinkBack  Thread Tools  Search this Thread  Display Modes 
July 7, 2020, 06:42 
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 
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 E04 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 

July 8, 2020, 12:04 

#2 
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 
Hi Somebody please help me


July 8, 2020, 12:23 

#3 
Senior Member
Join Date: Jun 2009
Posts: 1,365
Rep Power: 25 
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 1E04 (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?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

July 8, 2020, 13:23 

#4 
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 
Thank you very much for your response. I am looking to get a converged solution. I have set a residual target of 1E04 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 3741979. 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 

July 8, 2020, 14:03 

#5 
Senior Member
Join Date: Jun 2009
Posts: 1,365
Rep Power: 25 
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 wellconverged 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 CFDPost. 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
__________________
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 

July 8, 2020, 17:21 

#6 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20 
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 Rotorstatorinteraction. 

July 9, 2020, 02:41 

#7  
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 
Quote:
How can I plot the residuals in CFD post to locate where the maximum residual. can you please put some light on this 

July 9, 2020, 02:45 

#8  
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 
Quote:


July 9, 2020, 03:10 

#9 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20 
In Pre > Output control > Results, you can teel CFX to add the residual values to the results file.


July 9, 2020, 03:29 

#10 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20 
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 rotorstatorinteractions, 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. 

July 9, 2020, 05:38 

#11  
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 
Quote:
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 ? 

July 9, 2020, 05:42 

#12 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20 
Set them is opening, but put them far away.


July 9, 2020, 07:14 

#13 
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 

July 9, 2020, 09:28 

#14 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20 
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? 

July 9, 2020, 10:57 

#15  
New Member
Deepaksha K K
Join Date: Feb 2018
Location: Kochi
Posts: 11
Rep Power: 5 
Quote:
Very thankful to your every response and valuable time. It is very helpful to beginners like me. 

July 9, 2020, 11:30 

#16 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,324
Rep Power: 20 
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. 

July 9, 2020, 15:36 

#17 
Senior Member
Join Date: Jun 2009
Posts: 1,365
Rep Power: 25 
With GertJan'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 crosshair at the different locations where such value exists. Hope either methodology allows you to get a better understanding of where the solution is stuck
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Tags 
convergence, icem cfd meshing, mesh and grid 
Thread Tools  Search this Thread 
Display Modes  


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 