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

Contour discontinuities at interface(s) when plotting time-averaged variables

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

Like Tree2Likes
  • 1 Post By Stel
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 21, 2021, 09:07
Default Contour discontinuities at interface(s) when plotting time-averaged variables
  #1
New Member
 
Kenny Low
Join Date: Mar 2015
Posts: 3
Rep Power: 8
k.w.q.low is on a distinguished road
Hello everyone,

I'm currently simulating a centrifugal pump (multiple reference frame) using CFX 17.2. The pump (with 4 blades) was meshed as one part where all the nodes are connected at the rotor-stator interfaces (see interface figure). A steady-state simulation was initially conducted to provide an initial flow field for the transient simulation. The transient simulation was conducted for 10 rotations with 3 degrees of rotation per time step. After this, time-averaged values are activated (through transient statistics with arithmetic average) and conducted for an additional 5 rotations. However, when plotting the contours in CFD-post (particularly 'pressure' and 'velocity in stn frame'), I realised that there were contour discontinuities at the transient rotor-stator interface(s). I have tried various approaches and they have the similar outcomes:

1. time averaging for every time step (done 5 full rotations)

2. time averaging for every blade passage (done one full rotation with time averaging process conducted 4 times as the number of blades is 4)

3. time averaging for every full blade rotation (done 5 full rotations)

It would be great if anyone could please advise me on how to tackle this problem.

Thank you in advance.
Attached Images
File Type: png interface.png (58.8 KB, 11 views)
File Type: png discontinuity pressure.png (69.0 KB, 12 views)
File Type: png discontinuity vel.png (75.3 KB, 11 views)

Last edited by k.w.q.low; September 21, 2021 at 09:30. Reason: add figures for better clarification
k.w.q.low is offline   Reply With Quote

Old   September 21, 2021, 12:22
Default
  #2
Member
 
Henrique Stel
Join Date: Apr 2009
Location: Curitiba, Brazil
Posts: 92
Rep Power: 14
Stel is on a distinguished road
My feeling is that 5 full rotations for averaging is not enough for results to show a smooth transition for each variable through the interface in your case, or at least in the way that you are expecting to see it. It will probably sound confusing, but I'll try to explain why.

Since the instantaneous flow may vary a lot around the rotor periphery (you could confirm this to us, this could help us to better examine the problem), each particular rotor-stator position will have a different flow configuration. The interface flow will have a smooth transition at each given timestep because of the GGI model (or almost smooth, depending on how fine is the mesh and how accurate is the calculation), but since the rotor is being displaced in the " theta" direction any fluctuation will affect the averaging of both the impeller mesh results and the stator mesh results (which are now sliding one against each other). Thus, through the course of the averaging calculation, the adjacent mesh points on both sides of the interface are not being exposed to the same flow at every timestep as they were in the steady-state calculation. Because of this, I feel that this requires an extra amount of time for averaging compared to a situation where the flow is transient across a static-static interface, for example. Add to that the fact that the GGI model will have to interpolate the results for positions where the meshes on both sides of the interface don't match, and this could also require more sampling during the averaging.

After all, what you expect is that the flow from the rotor to the stator through the interface looks smooth independently of the final relative position between the rotor and the stator, right?
k.w.q.low likes this.
Stel is offline   Reply With Quote

Old   September 21, 2021, 18:06
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,835
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Umm, isn't this just because your mesh is too coarse? I can see the blockiness in your results, which means your mesh is very coarse. You will not get a "nice" smooth result with a coarse mesh.

So refine your mesh (reduce the edge length by a factor of at least 2, meaning your number of nodes will be 5x to 10x what it currently is) and try again. If that is still unacceptable then keep refining by another factor of 2 until you are happy with the results. This will result in a pretty big simulation, but that is why we run CFD on supercomputers
k.w.q.low 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   September 22, 2021, 01:56
Default
  #4
New Member
 
Kenny Low
Join Date: Mar 2015
Posts: 3
Rep Power: 8
k.w.q.low is on a distinguished road
Quote:
Originally Posted by Stel View Post
My feeling is that 5 full rotations for averaging is not enough for results to show a smooth transition for each variable through the interface in your case, or at least in the way that you are expecting to see it. It will probably sound confusing, but I'll try to explain why.

Since the instantaneous flow may vary a lot around the rotor periphery (you could confirm this to us, this could help us to better examine the problem), each particular rotor-stator position will have a different flow configuration. The interface flow will have a smooth transition at each given timestep because of the GGI model (or almost smooth, depending on how fine is the mesh and how accurate is the calculation), but since the rotor is being displaced in the " theta" direction any fluctuation will affect the averaging of both the impeller mesh results and the stator mesh results (which are now sliding one against each other). Thus, through the course of the averaging calculation, the adjacent mesh points on both sides of the interface are not being exposed to the same flow at every timestep as they were in the steady-state calculation. Because of this, I feel that this requires an extra amount of time for averaging compared to a situation where the flow is transient across a static-static interface, for example. Add to that the fact that the GGI model will have to interpolate the results for positions where the meshes on both sides of the interface don't match, and this could also require more sampling during the averaging.

After all, what you expect is that the flow from the rotor to the stator through the interface looks smooth independently of the final relative position between the rotor and the stator, right?
Hello Henrique,

Thank you for your explanation.

Yes, I understand what you mean and you might be correct. The reason I've done 5 rotations is based on what is being done in the literature (this pump is a benchmark blood pump). The range of time-averaging (no specifics) is between 2 (don't understand how can it be done) to 10 rotations. Nevertheless, I will try to simulate for more rotations. For example, starting from a converged periodic solution, I will do 20 rotations with time-averaging done for each pass of the four blades per revolution. This will give me 80 data sets and this will help in smoothing the contour.

On top of that, as Glenn said in your subsequent comment. The mesh that I'm currently using is a very coarse mesh (1.85 million cells) and this could have also contributed to the discontinuity. I will also conduct another one with a better mesh resolution.

This might take a while but if I have any further problems, I will come back to this post.

Thank you very much for taking time explaining this to me.

Kenny
k.w.q.low is offline   Reply With Quote

Old   September 22, 2021, 02:02
Default
  #5
New Member
 
Kenny Low
Join Date: Mar 2015
Posts: 3
Rep Power: 8
k.w.q.low is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Umm, isn't this just because your mesh is too coarse? I can see the blockiness in your results, which means your mesh is very coarse. You will not get a "nice" smooth result with a coarse mesh.

So refine your mesh (reduce the edge length by a factor of at least 2, meaning your number of nodes will be 5x to 10x what it currently is) and try again. If that is still unacceptable then keep refining by another factor of 2 until you are happy with the results. This will result in a pretty big simulation, but that is why we run CFD on supercomputers
Hello Glenn,

Thank you for highlighting this to me. Yes, the mesh that I'm currently using is a very coarse mesh (1.85 million cells) and this could have also contributed to the discontinuity. I was trying to debug the problem of the time-averaging process that I have specified in CFX. As per your suggestions, I will also conduct another one with a better mesh resolution to see whether it helps (I'm sure it will have a big impact as you said).

The simulation might take a while but if I have any further problems, I will come back to this post if you don't mind.

Thank you very much for taking time in providing the suggestions for me.

Kenny
k.w.q.low is offline   Reply With Quote

Old   September 22, 2021, 14:29
Default
  #6
Member
 
Henrique Stel
Join Date: Apr 2009
Location: Curitiba, Brazil
Posts: 92
Rep Power: 14
Stel is on a distinguished road
Most of the time, 5 full revolutions (obviously when starting the calculation with at least a steady-state solution as you did) are sufficient to calculate averages for most of the global quantities of interest (delta p, head, etc.), maybe that's why you usually find this in literature as a reference.

However, when it comes down to averaging velocity flow fields, every local fluctuation can greatly affect the average value at that point, thus requiring longer averaging periods until the whole pump average velocity flow field becomes steady. These local fluctuation regions can sometimes be so small that their effect on the global quantities are negligible, but the visual aspect of the average flow field, especially across rotor-stator interfaces, will look weird if the averaging is done through a short period of time.
Stel is offline   Reply With Quote

Old   September 22, 2021, 17:25
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,835
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I should point out that CFD-Post (and most other post processors) do not calculate things like contour post-processing objects across interfaces. They treat each side of the interface separately. This means there will always be a discontinuity at the interface. To minimise the effect until it is insignificant you need to a fine enough mesh - but there will still be a discontinuity, just a small one.
__________________
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
centrifugal pump, rotor stator interface, time average in cfx, transient cfx simulation

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
laplacianFoam with source term Herwig OpenFOAM Running, Solving & CFD 17 November 19, 2019 13:47
How to export time series of variables for one point? mary mor OpenFOAM Post-Processing 8 July 19, 2017 10:54
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM Running, Solving & CFD 8 March 28, 2016 11:08
Stuck in a Rut- interDyMFoam! xoitx OpenFOAM Running, Solving & CFD 14 March 25, 2016 07:09
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 04:03


All times are GMT -4. The time now is 07:45.