[Suman Sapkota]

Hello everyone;

I am simulating a pump flow. The geometry is a simple free impeller without volute casing. I encountered a situation in which the CFX gives error before starting any post particle tracking (after simulation). This happens when the particle size is very large 5 mm (min. mesh. size in X,Y,Z direction is 0.2, 0.2, 0.5 mm). My interest is not resolving the sub-viscous layer. So, after grid independent study i chose this mesh. Now, after some studies into particle tracking and meshing with the CFX, I did some sensitivity analysis with different particle sizes. When I simulated with particle size 0.035 mm (which is very less than the mesh size), I found that the particles near the refined mesh zone were predicted by the CFX. But then when the mesh size is 0.35 mm, the trajectory near the refined regions (especially the leading edge) vanishes.

[ghorrocks]

Are you doing Eularian particle model or Lagrangian particle tracking?

The particle size affects the particle mass and drag, which will affect the way the particle follows the flow. Is this what you mean?

[Suman Sapkota]

Thank you ghorrocks. I found it from your thread that particle diameter is modelled as point-wise. I am doing Lagrangian particle transport. Yes, increasing the diameter would affect the trajectory (more inertial force). I agree with it. Since we have established that point-wise modelled particles has no relation with the mesh size. My question is then: Why does it show error whenever I choose a diameter 5mm or, above. The flow simulation proceeds as normal but when the particle tracking begins, an error shows up. Err: Sig handler. Is there any limitations to the particle size on Lagrangian tracking? If there is, then what are the variables does it may depend on?

[ghorrocks]

Please post your output file as an attachment.

[Suman Sapkota]

After changing few parameters I found that the particles of diameter 5 mm almost does not hit the blade. As the particle diameter increases they tend to hit less on the blade surface which should not be true in the case of centrifugal pumps. heavier particles hit the leading edge and hub and shroud. but in my case the leading edge, where it is refined mesh to capture wall function (yplus~30) , the blade does not hit the leading edge, neither the trailing edge. I read from some papers and your discussion with julian K. regarding boundary layer resolution and particle size that other authors have also faced the same problem. I have a good result for flow that is in a suitable error range with experimental data but the problem of particle size and boundary layer resolution is what is bugging me. Are the particles with large size (in comparison to mesh resolution) captured with the small boundary layer resolution? I have tried by increasing from 10 to 15 layers to even 100 layers with the result of bad convergence. But i found particle hitting near the leading edge, but due to bad convergence the data was not physical. Can I say that the boundary layer resolution indeed affects the different diameter results in one way particle tracking?

[ghorrocks]

Don't forget that there is also the particle track settings to consider as well. You will want small integration time steps if the boundary layer flow is going to significantly affect your particles.

I would recommend that you do some validation and verification before proceeding. I would draw a simple test case which is easy to draw and mesh and test all the parameters to see their effects on whether particles penetrate the boundary layer and hit a wall or not. You should find a benchmark result so you can compare your results and work out how accurate you are. Once you have developed a procedure you know works with accuracy you are happy about then you should start simulating on your actual case.

[Suman Sapkota]

Thank you ghorrocks. Now, a simple question. I performed grid independent test of the pump and using the rules stated in "Journal of Fluids Engineering Editorial Policy", I got around 1.69 order accuracy for three grids. But I am using High resolution scheme and it fluctuates between 1 to 2 order accuracy. I do not have references to see if other researchers are getting the value around the same. I suspect it will be 2 because of the grid quality, convergence criteria (10^-5), etc. I wanted to know your view on this? Is 1.7 a good enough value for 2nd order accurate scheme in CFX specifically?

[ghorrocks]

If you are getting order 1.7 convergence on your mesh refinement then you can estimate what mesh is required for the accuracy you desire. It is not a matter of whether that is good enough or not.

[Suman Sapkota]

Dear Ghorrocks,
Thank you so much. With some digging, the particle track cannot approach the wall closer than dp/2, i.e. half the particle diameter. This would closer correspond to physics, since the particle track should represent the path of the particles center of mass. For larger particle diameter and very deep zoom into the BC layer this would appear like the particle track never really touches the wall surface but bounces in some distance from it. This makes sense to me.

Back to problem, This is a free impeller pump simulation with k-omega sst turbulence model. The first simulation is with boundary layer resolution (10^-6 m) order and particle diameter (10^-6 m order). This simulation predicted the particle track well and then I could have an assessment of the impact on impeller wall and subsequently determine erosion rate. But when I increase the particle diameter by an order (10^-5 m), even though the particle track is as expected, the region near the leading edge curvature is not eroded at all (no erosion rate density contour in leading edge). This is the region where the mesh is highly refined to capture the details of separation. When I increased the particle diameter again by an order (10^-4 m), the particles track appear to go close by the leading edge but none of them give the erosion rate density. In fact, the area near leading edge does not even experience erosion. This makes the erosion result look unphysical even though it is not. When I increased the diameter to 1 mm, then the particle track also shows going near the blade but still no impact at all. This time the particle do not even hit the suction and pressure side. When I increased the mesh size to 10 mm, the flow iteration took place as normal but as soon as it proceeded to the particle tracking, it experienced an error. I could confirm that in all cases the particle trajectory is very close to the blade which makes sense since they shout hit the blade, esp. at leading edge. But with both models (finnie and tabakoff in cfx), this problem persists. I tried making a small model to check, and I experienced the same particle size and boundary layer sensitivity.

I think that this might has to do with the way erosion rate model is implemented since we are not getting the contour we expect but the particle trajectory is as expected. I researched on the way models are implemented. The dimensionless erosion rate is should be zero if there is no erosion. The finnie model depend on the particle size through mass of particle. But how does it relate with bigger particles giving zero erosion rate density in one particular mesh. I could use your viewpoint.

[ghorrocks]

With Lagrangian particle track models you need enough particles to be statistically representative of the flow. For instance if 0.1% of particles hit the leading edge of the blade and you model 100 particles then the chances are that none of your modelled particles will hit the leading edge and you will think, incorrectly, that the erosion rate on the leading edge is zero. In fact all you need to do is increase the number of particles so you get a statistically signficant sample size and then you will get accurate erosion distributions.

In fact I would think this variable should be the subject of a sensitivity analysis to ensure you have enough particles modelled to be statistically significant.

[juven.sumen]

Hello Glenn,

I hope you are doing good. I have been encountering this problem that I have attached. The output file tells that there is error just as the flow simulation is completed. I could not attach the output file because the file size is large. I thought it was related disk size space available. I cleared the size and still shows this error. Is there a way to get around this?

[ghorrocks]

The error message is saying it has a problem with the size of the array to get the particle track data together. I have never seen this error and can only guess as to exactly what it means.

Check whether the slave has enough memory and disk space. Then check whether your particle tracks are doing what you want - are they really long? (then you might need to put a size limit on them) are there lots of them? (then you might need to reduce the number of particle tracks) is your particle track resolution too high? (then you might need to increase the particle track time step size)