Hello everyone. I am currently debugging a case with a strong swirling flow field within a complex geometry. I have been debugging for more than a month and have adjusted including mesher, STL files, boundary conditions, numerical methods, etc., but I still have not debugged it successfully so far, and I am very much looking forward to your help in solving these problems:
(1) A high speed zone as shown in figure 1 appears at the outlet in about 0.003s. The reason I use a fine mesh is because I have particles on the order of microns. When I use a coarse grid of 60, 12, 60, the phenomenon shown in Figure 1 is somewhat suppressed.
(2) A velocity inlet v=130m/s is used, but the velocity at the inlet is not 130 and there are many v=0 grids. There are also many v=0 grids at the wall.
(3) When using the turbulence model an error is reported. k and ε values tried for almost all magnitudes are not possible.
I have attached the case files, including another STL file without the elongated triangles. Again, I am begging for any help you can give me.
I would greatly appreciate it if the developers could assist me with this question, as it has been puzzling me for quite some time.
First, when you look at the velocity, it may be tricky because MFiX uses a staggered grid, so the velocity components are not stored at the same location. Some components can be zero for some cut cells if the cut is in the lower half of the cell.
Is the large velocity at the outlet a backflow? If so, you may need to extend the location of the outlet.
Thank you for your response, Jeff. I’ve tried re-simulating with an extended outlet, but the outlet velocity continues to increase over time and gets higher and higher. I don’t think it’s an issue with the outlet domain length because this phenomenon doesn’t occur with a coarse mesh. At this point, I’m really not sure how to proceed with debugging.I’ve attached the STL file for the extended exit.
Moreover, when I turn on the k-ε model, I get an error with DELH_Scalar=0.
@jeff.dietiker Sorry to bother you, Jeff.I tried extending the outlet and setting the small cell tolerance to 0.1. This alleviated the flow field at the outlet, and the time step stabilized near the maximum time step. However, there are still the following issues:
(1) The turbulence model reported an error due to DELH_Scalar=0
(2) When I added particles, they mysteriously disappeared. I adjusted all the particle collision parameters, but it still didn’t work. However, when I lowered the small cell tolerance, the situation improved. Upon observation, this may be because the particles escape from the ignored cells.
A small cell tolerance of 0.1 seems a bit large, maybe increasing the snapping tolerance could help.
- I have a fix for k-epsilon, please see attached. Copy the file into the project directory and rebuild the solver. I am not sure about the k and epsilon values you are using for IC and BC conditions though.
- The particles should see the stl facets, but if they are going too fast they may go through the wall. In this case, reducing the solids time step may help.
solve_k_epsilon_eq.f (14.0 KB)
Thank you very much for your reply, Jeff.
(1) I have also tried increasing the snapping tolerance, but then the second problem I mentioned above occurs.（When I added particles, they mysteriously disappeared. I adjusted all the particle collision parameters, but it still didn’t work. However, when I lowered the small cell tolerance, the situation improved. Upon observation, this may be because the particles escape from the ignored cells.）
(2) I will try the k-epsilon model you modified.
(3) I have already tried adjusting the time step factor for solids to 100, but it still does not work. What I mean is that when particles encounter pits like these, they suddenly disappear.I have attached a case with the DEM model in the attachment above.If you have time to check out my attachments, I would greatly appreciate it.
I see massive backflow in the latest case you attached CASE2-SOLID.zip:
Thank you very much for your reply, Jeff.
(1) I tried your modified turbulence model and when I adjusted the values of k and ε according to the equation, th e k-ε residuals are relatively low (<0.5), but the pressure residuals could not converge (>10). (k=6, ε=12000).
(2) How should this backflow phenomenon be suppressed? Is this related to the mesh?
(3) If we don’t discuss the backflow issue first, I’m still curious how to make the particles not suddenly disappear.
I think the most pressing issue is the backflow. You said extending the outlet location and increasing the small cut cell tolerance suppressed the backflow, can you show your results so I understand why I don’t see the same?
Now, with such large velocities and small particles, it is going to be pretty tough to run a DEM simulation. The solids time step will need to be very small so collisions are not missed.
I would not worry about k-epsilon at this point.
Sorry Jeff, I was only focusing on the absolute value of the velocity at the outlet and I checked again to see that there was still backflow. When I lengthened the exit position and increased the small cut cell tolerance, the absolute value of the velocity at the exit does not appear to have a higher and higher velocity until divergence as I first stated.
Sorry to bother you, Jeff. Is there any way to make the backflow go away and converge other than lengthening the outlet? In summary there are three current problems, in order of importance:
(1) Increasing the small cell tolerance or increasing the snap tolerance allows for gradual convergence, but backflow still occurs. If these two values are not increased, the pressure residuals do not even converge.
(2) The particles will encounter “small pits” and somehow disappear.
(3) The turbulence model does not report errors after correction, but the pressure residuals do not converge.
I don’t have a solution for the backflow. From what I can tell, the strong vortex creates suction in the vortex core that pulls the gas inward at the outlet. The PO outlet is meant to be used far from recirculation zones. Your setup looks like an ill-posed problem, but I don’t have experience with such high-speed flows in MFiX. Where is the gas supposed to exhaust?
Thank you very much for your reply, Jeff. The gas comes out of the bottom pipe as shown in the picture.
Can you setup a single phase flow with this geometry and see if you can get rid of the backflow?
I’m trying, Jeff. But I’m currently only able to run 16 threads for calculations, which is very slow. If we ignore the backflow issue for a moment, I’d still like to know why the particles hit the “pits” and disappear. This is different from the way some people in this forum say the particles disappear. This is because when the small cell tolerance or snap tolerance is very small, the number of particles disappearing inexplicably is very small, but the phenomenon still exists. But when the small cell tolerance or snap tolerance is increased, a lot of particles will disappear when they hit the “pits”, for example, if 200 particles hit the wall, more than 100 particles may disappear. And I have set the spring stiffness greater than 10000 and also increased the solid time step (Tcoll/Dt_solid=150) and tried to adjust other parameters as well. But all of them failed. If Jeff has time to try the case with DEM, I would appreciate it.
The particle velocity may reach 100 to 200 m/s. You can run a simple granular flow with a few particles hitting a wall at such velocities and adjust the parameters and time step until particles bounce off the wall instead of going through it. My guess is you need a tiny time step. As I said earlier, this may be a pretty tough simulation to run with DEM, especially if you only have 16 threads.
Regarding the backflow, I ran a test case with a very long (straight) exhaust pipe, and I don’t get any backflow, which suggest the BC location needs to be moved as far as possible from the recirculation zone. The middle plot below shows where recirculation occurs (in yellow) so the outlet must be downstream of the yellow region. Velocity vectors on the right show there is no backflow in this case.
Thank you very much Jeff for your reply, I will give it a try! Can you tell me if the very small time step is for a fluid time step or a solid time step? When I’ve debugged it successfully, I can do the calculations using a workstation, so I don’t have to worry about the cost of the calculations.
Solids time step (DTSOLID) used for the DEM loop. This is what is going to hold you off.
