## Fluids

#### Boundary Condition for Cone and Plate Viscometer

• Foelsche
Subscriber

Hello,

DESCRIPTION OF SIMULATION: I am trying to simulate a cone-and-plate viscometer (CPV) in Fluent, and I am having trouble with one of the boundary conditions. I am simulating the CPV from the CAD model attached. The petri dish will be seeded with cells on the bottom, and the cone will be driven by a motor. The circular edge of the cone is a set distance from the edge of the petri dish. When the fluid is placed in the petri dish, there will be some fluid that will ride up the side of the cone.

Also, I implemented a periodic boundary condition so that I only have to simulate a small slice of the CPV, as it is axisymmetric. I also have been driving the fluid with a cone speed of 10 rad/s with water as the fluid to start. Also assumed steady and incompressible. The holes in the petri dish will have tubing to replace the fluid inside.

MY ISSUE: I have been having trouble simulating the top portion of the fluid where the fluid will be exposed to the surrounding environmental conditions. I have tried various wall boundary conditions, and none of them are properly simulating a freely rotating fluid boundary condition. Whether I select stationary or moving wall, all of them result in this specific boundary as a stationary wall. I have tried both absolute and relative rotational velocity options, and neither does the trick. However, all of the other boundary conditions are working as expected.

Attached are the model of the cone and petri dish, as well as a velocity contour of the fluid. I only included the scale to show that the velocities are indeed correct according to v=w*r ( radius of cone is 0.045 m). As seen in the contour figure, the top part of the fluid is stationary. That is the issue I am trying to fix, as it should be free to rotate, not bounded as a stationary wall. The contour at the top wall should be a gradient from the highest speed to stationary, not all stationary. Thank you for any help.

• RK
Ansys Employee
Hello,
• Foelsche
Subscriber
These are the images I had attached
• Rob
Ansys Employee
If it's the free surface then symmetry might be a better choice.
• Foelsche
Subscriber
Hi Rob,
Thank you for that recommendation. I think that did the trick. I had thought for some reason that I had to have 2 defined boundaries to use the symmetry boundary, but I only assigned the 1 boundary to symmetry, and it worked. Thank you for your time and help! Here is the contour after I applied symmetry to the top boundary in case this could help anyone else.

• Rob
Ansys Employee
That looks better. Symmetry in the classic sense is to allow a mirror image of the results (we're talking Fluent 4 era). Now it's often used to mimic any frictionless surface that flow can't pass through.
Now you've got the result plot velocity vectors on the mid plane (angular position) and repeat for in-plane vectors.
• Foelsche
Subscriber
I have a follow-up question on the symmetry plane topic with respect to a dynamic mesh. If I were to implement a dynamic mesh onto the bottom (to move the bottom plane up and down), would I still be able to implement a symmetry boundary condition? I am thinking this might be problematic theoretically, as the fluid domain will be growing and shrinking, and that may cause continuity issues (the fluid is incompressible with a constant density).
• Rob
Ansys Employee
Sort of, if you change the volume without adding a vent (pressure outlet) the solver will do some of the these, fall over, fail to converge, lose mass and have a very strange pressure field. The latter three are most likely for small changes, as the change gets bigger the solution will diverge or return nonsense.
• Foelsche
Subscriber
I think I understand. The result was not much different, which is probably because the net displacement was not that high, but that makes sense to use a vent condition rather than symmetry when implementing a changing volume. Thank you for the help!
• Rob
Ansys Employee
You only want a small opening. You're welcome.