Reference frame vs direct motion
Hello,
I need to simulate a pipe rotating around its axis and see how the flow rate comes out through the outlets that are on the wall of the pipe.
My question is, the only difference between reference frame and direct rotation is when is it used? The reference frame in steady state and the direct rotation in transient simulations? Or can I use direct motion in steady state as well?
What are the other differences and how do I choose which one to use?
Attached is an example of what I would like to simulate.
Thank you.
Best Answer
-
Fededea said:
Thank you very much for the clarification.
This is just an example of what I want to simulate. Yes, the whole tube rotates, including the inlet and outlet. I want to try to learn how to simulate, for example, lubrication inside a rotating shaft with some nozzle.
You would probably want to use a time increment such that it takes maybe 10 time steps for the outlet nozzle to move one diameter - to get a good time-resolved solution. You would probably also need to apply the gravity body force - and activate hydrostatic pressure on the outlets, and use the same hydrostatic pressure origin for both of them.
0
Altair EmployeeAnswers
-
Mesh motion would need to be run transient - as the geometry/model is changing in time.
My general approach with reference frame:
1. If the rotating body (like impeller, etc) is the only thing that would cause unsteadiness in the flow/domain, then running transient with reference frame doesn't make much sense.
2. If there are other features in the domain that would cause transient flow, but you still don't want to run mesh motion in the rotating body, you could run that transient with a fixed-mesh reference frame approach. (But if already running transient - why not also rotate the mesh for the rotating body?)The rough theory behind reference frame is that the body is rotating fast enough such that the fluid behavior near the body is not changing much in time - any snapshot would look roughly the same. This holds quite well if there are no a-symmetric features in the geometry. If there are a-symmetric features near the rotating body, the blade-passing effects are missed with the fixed mesh reference frame approach - and the results can be quite different from running the rotating mesh transient approach. Also, if the angular velocity is quite slow, the effects of rotation are quite local to the blade surfaces, and the accuracy with running fixed mesh reference frame is again decreased.
Is that entire geometry in your image rotating - including the inlet and outlet tubes themselves? What is the physical/actual condition for this? What are you trying to learn from the simulation?
0 -
acupro_21778 said:
Mesh motion would need to be run transient - as the geometry/model is changing in time.
My general approach with reference frame:
1. If the rotating body (like impeller, etc) is the only thing that would cause unsteadiness in the flow/domain, then running transient with reference frame doesn't make much sense.
2. If there are other features in the domain that would cause transient flow, but you still don't want to run mesh motion in the rotating body, you could run that transient with a fixed-mesh reference frame approach. (But if already running transient - why not also rotate the mesh for the rotating body?)The rough theory behind reference frame is that the body is rotating fast enough such that the fluid behavior near the body is not changing much in time - any snapshot would look roughly the same. This holds quite well if there are no a-symmetric features in the geometry. If there are a-symmetric features near the rotating body, the blade-passing effects are missed with the fixed mesh reference frame approach - and the results can be quite different from running the rotating mesh transient approach. Also, if the angular velocity is quite slow, the effects of rotation are quite local to the blade surfaces, and the accuracy with running fixed mesh reference frame is again decreased.
Is that entire geometry in your image rotating - including the inlet and outlet tubes themselves? What is the physical/actual condition for this? What are you trying to learn from the simulation?
Thank you very much for the clarification.
This is just an example of what I want to simulate. Yes, the whole tube rotates, including the inlet and outlet. I want to try to learn how to simulate, for example, lubrication inside a rotating shaft with some nozzle.
0 -
Fededea said:
Thank you very much for the clarification.
This is just an example of what I want to simulate. Yes, the whole tube rotates, including the inlet and outlet. I want to try to learn how to simulate, for example, lubrication inside a rotating shaft with some nozzle.
You would probably want to use a time increment such that it takes maybe 10 time steps for the outlet nozzle to move one diameter - to get a good time-resolved solution. You would probably also need to apply the gravity body force - and activate hydrostatic pressure on the outlets, and use the same hydrostatic pressure origin for both of them.
0 -
acupro_21778 said:
You would probably want to use a time increment such that it takes maybe 10 time steps for the outlet nozzle to move one diameter - to get a good time-resolved solution. You would probably also need to apply the gravity body force - and activate hydrostatic pressure on the outlets, and use the same hydrostatic pressure origin for both of them.
Thank you very much for all the clarification. I will try with these settings.
regards
0