[dreamchaser]

Originally Posted by ghorrocks

Accuracy - If you are happy with 2.34N versus 2.44N then yes, it looks good. It depends on how accurate you need to be.

I do not like the justification your paper states. If you are not modelling cavitation it is true that the regions with pressure less than absolute zero are likely to have cavitated. However, the cavitation will then not behave as a simple single phase incompressible fluid - specifically the cavitation region is likely to be much larger than the negative pressure region in a single phase simulation.

So I strongly doubt the accuracy of the assumption that cavitation can be accounted for by ignoring negative absolute pressures. I would recommend you just work out the force over the whole thing, and if you have significant cavitation regions then you do a cavitation model to do it properly.

Hi Glenn,

*How would I know if I have significant cavitation regions?


*Regarding the negative pressure, can you explain what physically would happen if I did an experiment and actually spun this sphere against a flat plate? Based on the results, would the positive pressure push the plate outwards while the side with the negative pressure would cause the plate to collapse inwards? I imagine that this would not happen and that the plate would move away equally due to the pressure generated.
Just trying to understand the reasoning for taking the force over the whole wall.


*I used the function calculator (as you said) where I selected the force function and changed global to Y direction since I am interested in force in y direction. I applied the function to the whole wall and got a force that was very small 0.025 N.

As comparison, only using the force function on the converging part of the wall where the pressures were positive gave me a force of .137 N. What is the variable that is causing this major difference? Since the pressures are all negative on the diverging part of the wall, I assume that the force function applied over the entire wall should gave a similar result as only applying it to half of the wall. Unless the ‘viscous’ forces on the diverging part of the wall somehow reduces the entire force? However, I also did an area integral of pressure over the entire wall which also gave .025 N.

*However, using the force function over the entire wall gives a force that makes a lot more sense. For example, spinning the 3 inch radius sphere at a 100RPM and using the force function over the entire wall gives .025N as compared to .137N (which seems high). I am not sure how I justify that integrating over the whole wall is the correct way as opposed to just doing half of the wall. I assume that since I have not put in the Sommerfeld conditions into the simulation ( a boundary condition that states that the pressure is zero everywhere in the diverging part) where I make the pressure zero after the converging part, I have to integrate over the whole wall.


I just want to make sure I get the force correctly because this is the main objective of this project. The max pressure being generated is correct based on the analytical solution.

Thanks in advance for your advice and time

[ghorrocks]

How would I know if I have significant cavitation regions?

That depends on how accurate you want to be. If you do a simulation with a cavitation model then repeat it with the cavitation model off you will see the difference. But doing accurate cavitation models is difficult so this is no easy task.

Q2: I assume your bodies are rigid, and that the external faces are fixed in space. Then the fluid (cavitated or otherwise) applies a pressure and shear force on the cylinder, and this is reacted through the cylinder somehow (depends on the cylinder restraints). If there is a residual net force then the cylinder will accelerate in that direction.

Q3: That is because the forces are cancelling out across the object. I suspect torque might be a better measure that force.

[dreamchaser]

Originally Posted by ghorrocks

That depends on how accurate you want to be. If you do a simulation with a cavitation model then repeat it with the cavitation model off you will see the difference. But doing accurate cavitation models is difficult so this is no easy task.

Q2: I assume your bodies are rigid, and that the external faces are fixed in space. Then the fluid (cavitated or otherwise) applies a pressure and shear force on the cylinder, and this is reacted through the cylinder somehow (depends on the cylinder restraints). If there is a residual net force then the cylinder will accelerate in that direction.

Q3: That is because the forces are cancelling out across the object. I suspect torque might be a better measure that force.

Hi Glenn,

I am trying to correlate my results with an analytical solution. As I increased the RPM of the sphere, I noticed that taking the force over the whole wall was not canceling out anymore. I believe this is due to the fact that as the RPM increases, the absolute value of the maximum positive pressure starts to exceed the absolution value of the minimum negative pressure. I will run some more cases and compare the force result with the analytical and CFX results (force over half wall and full wall)

Comparing with the analaytical solution, I realize that my pressure was matching big gap distances and then began to deviate from the analytical solution as the gap distance decreased. In addition, overall my force calculation was off from the analytical solution. I believe that the correlation was not good was because my mesh at the wall is very poor. I have been importing a 2D mesh into CFX as a fluent mesh which extrudes the mesh some small distance. As a result, the mesh cells are very coarse at the wall giving a poor approximation of the force function compared with the analytical solution. Can this be a possible reason? Picture of Mesh is attached.

Would you suggest me to just do a 3D mesh (and set symmetry conditions on front and back wall) and increase the mesh elements in the extruded direction intead of doing a 2D mesh? I believe this will increase the number of elements on the area of the wall thus leading to a better approximation of the force function at the wall.

Please let me know if my reasoning makes sense.

Thanks

[dreamchaser]

Originally Posted by dreamchaser

Hi Glenn,

I am trying to correlate my results with an analytical solution. As I increased the RPM of the sphere, I noticed that taking the force over the whole wall was not canceling out anymore. I believe this is due to the fact that as the RPM increases, the absolute value of the maximum positive pressure starts to exceed the absolution value of the minimum negative pressure. I will run some more cases and compare the force result with the analytical and CFX results (force over half wall and full wall)

Comparing with the analaytical solution, I realize that my pressure was matching big gap distances and then began to deviate from the analytical solution as the gap distance decreased. In addition, overall my force calculation was off from the analytical solution. I believe that the correlation was not good was because my mesh at the wall is very poor. I have been importing a 2D mesh into CFX as a fluent mesh which extrudes the mesh some small distance. As a result, the mesh cells are very coarse at the wall giving a poor approximation of the force function compared with the analytical solution. Can this be a possible reason? Picture of Mesh is attached.

Would you suggest me to just do a 3D mesh (and set symmetry conditions on front and back wall) and increase the mesh elements in the extruded direction intead of doing a 2D mesh? I believe this will increase the number of elements on the area of the wall thus leading to a better approximation of the force function at the wall.

Please let me know if my reasoning makes sense.

Thanks

Picture of elements at wall is attached

[ghorrocks]

I believe this is due to the fact that as the RPM increases, the absolute value of the maximum positive pressure starts to exceed the absolution value of the minimum negative pressure.

I do not understand your reason. Can you explain it again? Can you show an image which shows want you explain?

[dreamchaser]

Originally Posted by ghorrocks

I do not understand your reason. Can you explain it again? Can you show an image which shows want you explain?

I attached a picture of the pressure as I increased the RPM. As a note, the max pressure is matching the analytical solution. I believe the pressure distribution is not symmetrical due to the geometry of my domain. As the pressure is diverging and going negative, the fluid is then converging again as it approaches the subsequent converging gap.

Maximum pressure at 100RPM is 10139.300000 and minimum pressure is -9457.930000

Maximum pressure at 500RPM is 59052.300000 and minimum pressure is -43299.800000

Maximum pressure at 1000RPM is 135191.000000 and minimum pressure is -81274.700000

[ghorrocks]

You mean that as the speed increases there will come a time when the fluid cavitates? Yes, that would happen. And yes, if the flow cavitates then it will not be symmetric-ish.