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!

I don't know in which country you live, but here we define horizontal as perpendicular to gravity, see picture.

Vertical outlet conditions as you tend to use are killing your simulation.

The geometry that you added lately, as connected to the screw, is not necessary in my opinion.

And important: apply wall boundary conditions for the 4 surfaces between air and water outlet.
No matter if this is not in agreement with reality. I suspect that it is not of interest how the water leaves the simulation, not? At least, it won't affect the performance of your generator.

Dear Gert,

Hope now these boundary conditions are OK. Are they?

Thank You for your advice.

The bottom outlet should have water=1 and air =0.
Your initial guess should contain a certain water level, as you did in your setups as shown previously.

Remember, these kind of simulations remain rather difficult and are suspectible to divergence quite fast. So, don't give up fast, make back ups, check the flow once in a while, see where it fails. etc. I have 20 years of experience and would already consider this simulation as a challenge.

If it fails again, you might need to make a horizontal inlet as well. Just add a 90 bend where the water is coming from below. This will prevent air trying to enter your inlet.
An other source of error you might bump into is that your water outlet is too close to the pipe at the end of your screw. Alternatively add a few meters: make the bassin deeper.

Dear Gert,

Ok, I adjust the volume faction as you said and the bottom opening pressure as I expressed earlier. Is it OK?

Thank you!

Antother thing: It looks like you now have the end of the outletpipe flush with the air outlet: bad idea. I would extend the outlet pipe a bit into the air above the water, making a clear distincting between pipe and air outlet.

What CFX-version are you running?

Dear Gert,

Are these boundaries OK now? I am doubtful about bottom pressure. How can I indicate the bottom boundary?

The CFX version is Ansys CFX 17.2

Impossible to say from here. Important is to check it with your initial guess in CFD-Post. I would start you simulation with the expert parameter: backup file at zero iteration (out of my head, somehting like that)
This will write your initial guess to a backup file, allowing you to see (in Post) if everything is setup correctly. Initial guess and boundary conditions!

In earlier version you had to include the hydrostatic pressure in the initial guess and on the boundaries. At some version, CFX changed this. Hydrostatic pressure got included in the reference pressure. I don't know which version they changed this.
So, either you can get away with pressure = 0 everywhere (CFX will incorporate the hydrostatic pressure for you), or you have to specify and intialise with hyrdrostatic pressure.

Bottomline: check your settings in Post with the backup file at iteration = zero

Dear all,
 

I have tried many times reading, again and again, your suggestion.

In the end, I was asked to do validation on the article of "Computational fluid dynamics modelling for the designed of Archimedes Screw Generator" This CFD work has done using the OpenForm.

In validation CFD work;

When I use free slip wall condition to rotating domain walls (Blade wall, Shaft wall and Trough wall) it working well for even small-time step 0.002s.

But in the real application, walls are usually no-slip and the trough is non-rotation. Therefore, using the previous initial results then I try no-slip wall condition; and the trough wall defines as wall velocity > rotating wall > 0rad/s.
This conditions working well for 0.002s time step.

After I notice in CFX modelling guide, to make trough wall stationary, the option is counter-rotating wall.
But when I use that option the simulation gets bad and stopped resulting fatal overflow error in 0.002s time step.

Is it OK to use counter-rotating wall?

For your reference here I attached the picture of blade, shaft and trough.

There is no fundamental problem with counter rotating walls in rotating domains. If there was the option would not be available.

So the fact that you are having problems with it means there is some problem with your simulation to create this problem. You are going to have to do a debugging exercise to find it - output the residuals to your output file and save a transient results file just before it crashes. Have a look at the residuals to find the problem area. That should give you a hint of where to look.

In your case two things I would consider important is double precision numerics and making the time step smaller.

Dear all,
 

I was glad to inform you that for 0.002s time step validation was run successfully.

First I use free slip wall (Blade, shaft and trough) to make the simulation stable. - figure 1

Then using the above initial file, a simulation was run for no-slip wall condition, but the trough wall is 0rad/s rotation with respect to local co-ordinate. (In global coordinates trough wall have same rotational velocity as rotational domain) -figure 2

Finally using the latest initial file, a simulation was run for no-slip wall condition, with stationary trough wall. (Use counter-rotating wall option) –figure 3

I would like to thank everyone who helps me with my issues.

Now I am going to run the designed model having the same CFX set up as validation. Hope it is running well. Further, I try to make the simulation more reliable. I will let you know about the progress.

If there any suggestions for further improvement, I kindly request from you all as those suggestions are valuable for my further studies.