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.