[tango711]

Hello,

I am new to the world of CFD and I have to say that this forum has been a great asset in over coming many of the issues I had faced, many thanks are due.

Up to now I have been stuck in a problem and cannot find the solution to here, maybe someone has had previous experience with this. I am attempting to model the flow in a certain domain, where the inner wall should be rotating and the outer wall should be stationary as seen in Figure 1.

Thus I applied a rotating boundary condition at the rpm I want to the parts being rotated, but I get an error of the tangential velocity being normal to a surface, which is true as can be seen in the cross section of the part in Figure 2 and a close up in Figure 3.

To try to fix this, I made the whole domain rotate and applied a counter rotating wall condition on the outer wall, thus making it stationary in the absolute frame. In CFX Post this seems to work, as when I plot an isosurface of zero velocity with respect to the stationary frame I get what I expect that the wall has zero velocity (Figure 4 and Figure 5 show part before and after isosurface plot, respectively).

Will this give me an accurate model?
Is there another way of going around doing this?

Please let me know,

Thank you

[tango711]

To validate what I have done I am taking a simple case of two concentric cylinders and see what happens where when I rotate the domain (Figure A) and apply a counter rotating condition on the outer wall. I get the same results with the isosurface (Figure B)

I plot the velocity along the line shown in Figure C, and I get a solution that makes sense with the expected tangential velocity at the inner surface and almost zero at the outer surface as seen in Figure D.

However, when I increase the diameter of the cylinders keeping the gaps constant and plot the same line as in Figure C I get the following plot as seen in Figure E.

[lffabiani]

Tango 771,

Isn't this a case of a rotating DOMAIN? What boundary conditions are you using?

Best regards

[tango711]

Thanks for the reply lffabiani,

No in reality I this domain is not rotating, only the inner wall sufraces. This is a sub domain of a larger domain which makes up a pump seal.

My inlet and outlet are actually on another subdomin, this part is connected to the rest of the domains through interfaces (frozen rotor interface when needed) above and below it. Figure 6 shows the whole computational domain with this specific part highlighted in green. All surfaces except the outer wall should be rotating.

Please let me know if this helps.

Thanks

[JoseptDavid]

Hello Im David,

I am studing my master degrees and I am relatively new in CFD tool, my case is the following:

I need to simulate a struture with a fluid impacting it, I am new in AUTODYN and my english isnt very clear, but i will try to explain me:

In a Natural Channel Condition, I have a concrete matress on the Channel, I need doing to flow a water into the channel and I want to observe the structural displacement of the matress and its displacements. Is that possible with AUTODYN? and if that is possible i'd appreciate your help.

Thanks and regards

[lffabiani]

tango711,

Just to be clear, what is the error? Does CFX crashes or you are saying that the simulation is not correct?

Can you plot a cross-section plane with the tangential velocity and vectors?

Best regards

[tango711]

Originally Posted by lffabiani

tango711,

Just to be clear, what is the error? Does CFX crashes or you are saying that the simulation is not correct?

Can you plot a cross-section plane with the tangential velocity and vectors?

Best regards

Yes, it is the second part. I am wondering if the simulation would be correct if instead of applying a rotational wall boundary condition on the inner wall, I have the whole domain rotate and apply to a counter rotating wall boundary condition on the outer wall.

As for my second post, I was checking to see if what I did make sense so I applied the same conditions to two concentric cylinders, but I got strange results. I attached cross-sections with the tangential velocities in Figure F for a small scale which works, and Figure G which is a large scale, and as you can see half way between the two cylinders the vectors change direction, I am not sure why.

Thank you for your time

[lffabiani]

My advice would be to:

1- Turbulence model. Is it the right one?

2- Verify your mesh. Check the Y+ values on walls with the recommended for the turbulence model, size sensitivity check.

3- Verify the convergence (http://www.cfd-online.com/Wiki/Ansys_FAQ)

Hope it helps!

[tango711]

Originally Posted by lffabiani

My advice would be to:

1- Turbulence model. Is it the right one?

2- Verify your mesh. Check the Y+ values on walls with the recommended for the turbulence model, size sensitivity check.

3- Verify the convergence (http://www.cfd-online.com/Wiki/Ansys_FAQ)

Hope it helps!

Thank you for your advice Luis,

I am checking it in the laminar case. However, for when I try the large scale (the one with funny results) the solver finishes normally within 5 iterations. While the smaller scale one took around 60 iterations.

Is the quick convergence of the large scale case an issue? I cannot find fast convergence problems in the link you provided or in other parts of the forum.

Thank you,

[flotus1]

5 Iterations until "convergence" is very unusual.
How did you check if your simulation is converged?

Run the case for a few hundred iterations and see if the results are more plausible.

[lffabiani]

Alexander is right. Try setting the minimum iterations to 80 and check if the results change

[tango711]

Originally Posted by flotus1

5 Iterations until "convergence" is very unusual.
How did you check if your simulation is converged?

Run the case for a few hundred iterations and see if the results are more plausible.

Hello Alexander,

I set my minimum iterations to 100 and I ended up with stranger results than previously; now the vectors change direction twice as in Figure H.

Would having large diameter concentric cylinders be affecting this somehow through the shearing of fluid?

What do you guys think?

Many thanks,

[flotus1]

Would you mind showing the residuals?
The result in your last picture does not look like a converged solution.

If I get you right, the inner and outer wall of your domain are counter-rotating. For this kind of shear driven flow, slow convergence is a typical issue.
It is possible that more than thousand Iterations are necessary.

BTW: if you upload your pictures in a picture format, then it is much easier to open them.

[tango711]

Originally Posted by flotus1

Would you mind showing the residuals?
The result in your last picture does not look like a converged solution.

If I get you right, the inner and outer wall of your domain are counter-rotating. For this kind of shear driven flow, slow convergence is a typical issue.
It is possible that more than thousand Iterations are necessary.

BTW: if you upload your pictures in a picture format, then it is much easier to open them.

Yes, the whole domain is rotating including the inner wall and I applied a counter rotating wall in the outer wall so that I can model it as if it were stationary.

I am doing this as a check, because in my actual domain, I want to have the inner wall rotating, but cannot due to a "tangential velocity normal to a wall" error, which is because I have a radial wall. Thus I am trying to see if using this method, will achieve similar results.

Hope this clears it a bit more.

I have also attached the summary of the run. Sorry for the pdf files, I will attach in JPEGs from now on.

Thanks again,

[gbrajtm]

Hi,

I am doing the similar analysis. I created and did analysis, but in post processing, the inner wall is not rotating.
I am able to see contours at last time steps only, no contours are showing for other steps. My BC's are, the inner wall is rotational and the outer wall is stationary. I have attached CCL for reference.
Please let me know whether I missed out some input setups.

Thanks

[Gert-Jan]

Your CCL shows:


OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
TRANSIENT RESULTS: Transient Results 1
File Compression Level = Default
Include Mesh = No
Option = Selected Variables
Output Boundary Flows = All
Output Variable Operators = All
Output Variables List = Pressure,Total Pressure,Total Mesh Displacement
OUTPUT FREQUENCY:
Option = Every Timestep
END
END
END


So, in all timesteps, you only save the variables Pressure,Total Pressure,Total Mesh Displacement. You should add 'Velocity' to be able to plot this variable.

[gbrajtm]

yea, Thanks. Now I am getting results!!!