[cfd seeker]

Originally Posted by ghorrocks

Your description of the system appears to suggest that there should be an outlet in your system to a hydraulic actuator, or one of the walls in your modelled system should move as it is the actuator. If this is correct then you have an inlet and somewhere for the fluid to go and your model makes sense.

Yes this is a hydraulic actuator and one of the walls moves vertically upwards because of the high pressure oil. After the actuator lifts the external system it will return back (moves vertically down) under the action of gravity and the oil will move back through the inlet into the reservoir. So on the return stroke of actuator the inlet will become outlet. The things is, at first I don't want to do the moving mesh/dynamic mesh analysis. I just want to do the analsysis of system in stationary state at the start configuartion to know that when oil enters the actuator and it reaches the actuation surfaceand sealing rings (the surfaces maked as red in the last post) how big are the pressure losses. I suppose I have made myself clear.

Is it possible to do such an analysis? Or is there any alternate if I want to do the analysis of the system in stationary state?

[ghorrocks]

Yes, you can do this analysis but you need to define it properly before you will get anything sensible. You have to model the actuator somehow, as the oil needs somewhere to go otherwise nothing happens (as has been described earlier in this thread).

So you need to either model the motion of the actuator or put in an outlet boundary to allow oil to exit the domain. The outlet is easiest to apply - work out the mass flow rate which the actuator motion generates, and apply this mass flow rate as your outlet boundary (or your inlet). Then you have an inlet and an outlet and a flow will be generated.

[cfd seeker]

Originally Posted by ghorrocks

Yes, you can do this analysis but you need to define it properly before you will get anything sensible. You have to model the actuator somehow, as the oil needs somewhere to go otherwise nothing happens (as has been described earlier in this thread).

So you need to either model the motion of the actuator or put in an outlet boundary to allow oil to exit the domain. The outlet is easiest to apply - work out the mass flow rate which the actuator motion generates, and apply this mass flow rate as your outlet boundary (or your inlet). Then you have an inlet and an outlet and a flow will be generated.

Hi Glenn,

Case1: if I just model the movement of actuator in one direction (just the lifting stroke, no return stroke) and without any Outlet then will it be possible to model this problem?

Case2: If I choose to model the Outlet without any movement of actuator then in this case will it be sensible to extend the actuator lifting surface and sealing rings to 20*diameters and apply the mass flow rate or outlet pressure (atmospheric pressure) B.C? I am not sure if I will get the real time scenario by doing so? What's your opinion?

Regards

[ghorrocks]

Both approaches can work and are numerically well posed. But whether the approaches are suitable for what you are modelling and and what you are trying to do depends on many factors you have not described, like what you are intending to do with the information from the model, how accurate it needs to be, what system this modelled device is part of and its characteristics and so on.

[cfd seeker]

Originally Posted by ghorrocks

Both approaches can work and are numerically well posed. But whether the approaches are suitable for what you are modelling and and what you are trying to do depends on many factors you have not described, like what you are intending to do with the information from the model, how accurate it needs to be, what system this modelled device is part of and its characteristics and so on.

Hi Glenn,

i want to double confirm it. The first approach with moving wall and without any Outlet is numerically well-posed? Right?

The system is a hydraulic actuator as you already knwo. Its design needs to be changed little bit, so the current design needs to be accessed so that to see the pressure losses in the system. Also the forces in the sytem later needs to be analysed so that the other involved parts would be changed/optmized accordingly.

[ghorrocks]

Rather than asking me whether it is well posed it is better for you to understand the concept and confirm it for yourself. But in short there needs to be somewhere for the fluid to go. An inlet and an outlet will do this, and so will an inlet and a moving boundary (think blowing up a balloon).

[cfd seeker]

Now I am simulating this problem with moving wall now. Wall is also moving and simulation is running fine. But when i check the in-between results I can't see any change in pressure. Pressure plotted on the symmetry plane as shown in the attached figure is same as specified on the inlet. Also the velocity is zero. I don't know what's wrong in the simulation. Any suggestions?

Total_Pressure_Symmetry.jpg

Velocity_Symmetry.jpg

Solver_Convergence.jpg

[ghorrocks]

Are you sure your motion is correct? Use the debugging technique here (https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F) to check your mesh motion is correct.

I notice you applied a mesh motion onto the inlet boundary. That does not sound correct.

[cfd seeker]

Are you sure your motion is correct?

Yes I am sure that the motion is correct as I have checked the transient file at different time steps and it showed that the wall is moving correctly and in right direction.

I notice you applied a mesh motion onto the inlet boundary. That does not sound correct

Yes Inlet is also translating upwards and it is like this in reality. The motion of actuator I tried to explain in this thread.
Dynamic Mesh Model - Simple Question

[ghorrocks]

Applying moving mesh to inlets and outlets is going to cause problems. I have had a quick look at the other thread and do not understand why you think a moving inlet is required.

[cfd seeker]

Originally Posted by ghorrocks

Applying moving mesh to inlets and outlets is going to cause problems. I have had a quick look at the other thread and do not understand why you think a moving inlet is required.

Because the whole of left portion of domain i.e. Adjuster of Actuator (in real system) is translating vertically upwards. The Inlet walls are actually part of the adjuster, so they move up also.

[ghorrocks]

Please post an image showing what faces you have defined motion on, and what direct they move in.

Things will work a lot better if you keep the inlet stationary and move the rest of the actuator to follow the motion.

[cfd seeker]

Please look in the attached figure how adjuster is sliding along so that the Inlet also moves. Actually Inlet is part of adjuster so it always moves. I hope from the figure it's clear to understand.

Actuator.jpg

[ghorrocks]

Please show what faces are moving and what direction they are moving in. I do not understand what is happening from that image.

[cfd seeker]

Hi,

sorry i forgot to mention that all the green walls in the image are moving vertically upwards and also the blue Inlet. All other walls are stationary.

[ghorrocks]

It appears the inlet does not have motion normal to the boundary, so that is OK. mesh motion tangential to an inlet boundary is OK.

On your question about convergence: Have you done the normal things to improve convergence?
* Smaller time step
* double precision numerics
* better mesh quality
* better initial conditions

[cfd seeker]

Hi,

convergence is there as the residuals are droping. But the problem is I can't see any pressure loss. Flow in whole of domian stays at the Inlet pressure.

I am not sure if it's possible to solve this problem this way i.e. No Outlet and moving wall. As the domain size is increasing every time step and the flow is entering at the same pressure.

[ghorrocks]

It is possible to have flow driven by a moving mesh and an inlet. I have done it many times. There is some problem with your simulation.

Your images show some pressure variation and some velocity. So the flow is just starting up, isn't it?

[cfd seeker]

Ok I will let the simulation to run for longer time and see what happens.

[cfd seeker]

Originally Posted by ghorrocks

It is possible to have flow driven by a moving mesh and an inlet. I have done it many times. There is some problem with your simulation.

Your images show some pressure variation and some velocity. So the flow is just starting up, isn't it?

Another thing which I noticed from the simulation is that at the Inlet mass flow rate from simulation is 0.0000122 kg/s whereas the actual mass flow rate at Inlet is 0.0045 kg/s. I am using Total Pressure B.C. What could be the reason for that?

In CFX i can only specify one value as a B.C. How mass flow rate or velocity is calculated in CFX when there is just one Inlet with pressure information on it?