Archimedes Screw Generator
 

Hello!
(Reducing time step make solver fail, why?)

I am doing simulation on ASG in Ansys CFX. I created quality Hexa mesh using ICEM and set up in CFX considering the gravity flow. Since the rotational axis is not parallel to the gravity axis unable to do steady-state simulation. Therefore I did a transient simulation with 0.1s time step.

Since the screw rotational speed is 53rpm I tried to reduce the time step further to 0.05s after it converges under 0.1s time step. the first few iterations are going well and at some point, solver failed showing fatal overflow error.

First work through the issues discussed on the FAQ: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

Dear Mr.Horrocks,
Thank you for the link, and I have read it again and again.
I think;
1) the physics of the simulation set up correctly
2) the mesh is high quality
since it solver complete run for 0.1s time step.
3) the initial condition is already 0.1s time step calculation
4) double precision is already on
5) I tried with 0.05s time step from the beginning the solver fails even without converging. Therefore I use 0.1s for beginning and reduce time step 0.05s after converging. Error happens!!!

Do you know how to find a good time step for buoyancy-driven rotational flow?

The overflow error means your model is very numerically unstable. When you reduce the time step size you can resolve finer transient flow features which can lead to a reduction in numerical stability. This is a possible mechanism by which reducing the time step causes divergence.

In this case you need to improve the numerical stability. If you are sure you are modelling it correctly the next thing to look at is the mesh quality. A higher quality mesh will improve numerical stability, so even though your model converges with the existing mesh at the larger time step improving mesh quality is an important factor in resolving this problem.

Dear Sir,

Here I attached my basic mesh details. Under the 0.1s time step, the RMS Courant number is about 26. According to the courant definition if I may reduce the size of elements further it results in high courant number. But reducing the time step also reduces the courant #. I was read for better solution courant # is about 1.

Since I use the K-epsilon turbulence model I feel my mesh quality is enough.

Thank you!

:) I would not have mentioned it unless it was an issue. Improving mesh quality always helps, even when the simulation is already converging as it will then converge better. But yours is not even converging so you definitely would be helped by improving mesh quality.

But after seeing your geometry I think I see other problems. have you got an opening boundary on the top of this device? It is very close to the screw top, and I presume you have a GGI linking the screw to the inlet tube. Having an opening so close to a GGI and perpendicular to the flow direction is going to be numerically unstable. I would recommend you move this boundary further away from the important bit of your geometry, it will greatly improve your numerical stability.

Dear sir,

Thank you for your reply and now I am working to make my opening bit away from the screw. I may let you know as soon as I finish that. Thank you very much, for the important detail!:)

Like Glenn said...... having the outlet in a vertical position like this is troublessome. I always make the outlet for water in horizontal position, and an opening for air at the top. Then the pressure definition for the water part is clear, making the simulation much more stable.

Dear Gert-Jan,

I have considered your opinion and now I model a down channel with a horizontal opening. As well as I made my top opening away from the rotating domain. Now I am working on the problem. as soon as it completes I let you know.

Thank you very much for your advice.

Dear Glenn and Gert;

Thank you for the advice! but the problem seems to be same!!!

I have made my top opening away from the rotating domain (Screw) as figure 1. And I modify the simulation using the outflow channel and make the horizontal opening too. (the Previous outlet is an opening from rotating domain directly)

Solver manager monitoring graph is illustrated in figure 2.

Firstly, I tried to run having 0.05s time step at the beginning. But without converging the overflow error occur. Then I tried with 0.1s time step at the beginning and after converging I reduce the time step 0.07s. Having increased the power it converges again. Then I further reduce the time step to 0.05s. On the way to convergence the overflow error occurs.

**My monitor variables are torque on 2blade sides, hence the net torque and the power

Please advise; what shall I do?

The source of your error can be anything.
It could be that it has to do with the outlet. But we are not sure.
Therefore we advised to create a top outlet for air (orientation is less relevant) and a horizontal bottom outlet for water.
I still see a vertical outlet for water at the right hand side, not? Or am I mistaken?

Please make it horizontal at the bottom side.

Alternatively create a backup file at the timestep before it crashes. Then open it in post to find out where the problem is. Look for unrealistic velocities and pressures.......

I have marked up an image with my suggestions.

Attachment 73644

In addition to Gert-Jan's suggestions I recommend you include the residuals in the results file and view the residuals in CFD-Post. This will show you the areas of high residuals which are the areas it is having convergence problems. This will tell you what you need to focus on.

Dear Glenn and Gert;

Thank you for your advice.

Since I could not define my boundary condition, here I attached detail picture.

As you said, now I am going to run the simulation having the back-up and view it in CFD post. Further, I will try a simulation having a top channel opening away as you show in the previous attachment.

Dear all,

Here I observe where the fatal overflow happen.

I ran the simulation (boundary condition as attached picture) and I stopped my run at the moment where the error happens. Then I observe the CFD- post and I found there is a backflow (Water flow against the usual flowing direction, beginning from the outlet where the boundary condition is as opening with 0Pa).

For more details refer to the pictures of water volume fraction variation, velocity and pressure variation in water volume.

How can we overcome this condition? Am I want to improve my outlet condition?

What is wrong with my suggestion as posted on November 29th at 12:11?
Why didn't you try this? Is it unclear?

And you appear to have ignored my advice about moving the opening boundary back further as well.

Your latest images appear to show that the top side of the screw is also an opening. This will also be a convergence problem, you are going to have to connect a stationary domain to that via a GGI and put the opening boundary further away. In short, you want the flow to be going perpendicular to opening boundaries. If it has much of a tangential component it will be numerically unstable. This also links into Gert's suggestion, it means the flow on the top opening boundary in his suggestion is perpendicular to the boundary.

Your comment seems to suggest that it crashes when you get some back flow - this is exactly what I would expect when some of the back flow touches the opening boundary tangentially.

Dear Gert-Jan,

I am sorry that I could not mention what I have done as you said. I make my outlet opening horizontal as shown on December 3, 2019, 20:20 post.

But the same problem arose when running the simulation, as attached in this post. Unfortunately, I couldn't make a backup file or stop the simulation before it fails, therefore I could not observe the problem.

I assumed the problem was the negative pressure built-up inside the screw since it starts the backflow. Therefore I make the top part of the screw as opening while the bottom part present as wall (As shown in the previous post).

As you advise earlier again I am trying to re-do with the horizontal out as opening.

Sorry about my mistake and hope your support further.

Dear Ghorrocks,

Thank you for the advice. Now I am going to make my every opening perpendicular and horizontal. This may be the problem.

As soon as I finished the modelling I may update the progress.

Thank you and hope your advice further!

Dear sir,

Here my new modal I made today. I named the boundary conditions, if there are any suggestions to modify please let me know. It may help me to do a fine simulation.

Thank you!