[k.w.q.low]

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.

[Stel]

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?

[ghorrocks]

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]

Originally Posted by Stel

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]

Originally Posted by ghorrocks

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

[Stel]

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.

[ghorrocks]

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.