[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?

Thta would be really interesting to know that if Total pressure B.C is used in such a simulation (one inlet, no outlet and moving wall) then from the solver will get the information about the velocities?

[Lance]

I dont get it. What is your question/problem?
You have a single inlet, no outlet and a domain that changes in size?
Given an incompressible fluid you must have a flow rate at the inlet, which is determined by the time rate of change of domain volume. If the flow rate is wrong (compared to what?) then your domain volume change (wall motion) is changing too slow or fast.

[cfd seeker]

You have a single inlet, no outlet and a domain that changes in size?

Yes

Given an incompressible fluid you must have a flow rate at the inlet, which is determined by the time rate of change of domain volume. If the flow rate is wrong (compared to what?) then your domain volume change (wall motion) is changing too slow or fast

No, flow rate is not determined by the time rate of change of domain volume. Mass flow rate is dependent on the pump. Actually the flow coming out from the pump at particular mass flow rate and at particular pressure generates the pressure inside actuator which forces the actuator to lift upwards.

[Lance]

Originally Posted by cfd seeker

No, flow rate is not determined by the time rate of change of domain volume. Mass flow rate is dependent on the pump. Actually the flow coming out from the pump at particular mass flow rate and at particular pressure generates the pressure inside actuator which forces the actuator to lift upwards.

But that is not what you are modeling if you prescribe the wall motion... You can have any pressure at the inlet, but the mass flow rate is going to depend on the volume change of the domain when you prescribe the wall motion.

[cfd seeker]

Originally Posted by Lance

But that is not what you are modeling if you prescribe the wall motion... You can have any pressure at the inlet, but the mass flow rate is going to depend on the volume change of the domain when you prescribe the wall motion.

Ok. But in reality the flow enters at particular pressure and mass flow rate which generates pressure inside domain and this generated pressures forces the domian walls to move for a particular distance in a particular time. Can this be modelled? If yes how?

[Lance]

Yes,

either with a coupling to a solid solver ("2-way" FSI)

or

using the generated pressures and knowledge about how much displacement that would result in, prescribe the displament using a CEL expression.

[cfd seeker]

Originally Posted by Lance

using the generated pressures and knowledge about how much displacement that would result in, prescribe the displament using a CEL expression.

I am already specifying the displacement on the walls using expression (using d = V*t) but I know only the pressure at the Inlet. Thr purpose of the simulation is to determine the presure loss of flow till it reaches the displaced surfaces/moving walls. So what could be done in this case?

[cfd seeker]

Originally Posted by Lance

Yes,
using the generated pressures and knowledge about how much displacement that would result in, prescribe the displament using a CEL expression.

I was already modelling this by specifying the dispalcement on the moving walls using expression (d = V*t, "t" being the simulation time). But in your previous comment you said this problem can't be modelled like this. Can you please elaborate further on this?

Purpose is to study the pressure losses till the flow reaches the lifting surface/moving walls.

[Lance]

If you prescribe the motion by d = v*t (assuming v is velocity?) then I assume you know the velocity the wall moving with? Then, if the mass flow at the inlet is too low/high, then this velocity is too low/high.

If the goal of your model is to get the pressure drop from inlet to moving wall, then I would run a bunch of simulations with different prescribed displacement velocities and check the mass flow rate and pressure drop.

You can prescribe the motion of a surface as a function of almost anything, including pressure, force, etc. Use CEL expressions (e.g. areaAve(pressure)@surface). Of course this would require knowledge about mass, external forces, etc. In earlier versions of CFX (v11 maybe?) there used to be a good example of how this was solved on a ball check valve, but it has now been replaced by the rigid body solver.

Anyway, it sounds like you need to take a step back and think through what you are interested in and what you are actually modelling.

[cfd seeker]

If you prescribe the motion by d = v*t (assuming v is velocity?) then I assume you know the velocity the wall moving with? Then, if the mass flow at the inlet is too low/high, then this velocity is too low/high.

Wall velocity is correct as the stroke length of actuator and the time it takes to complete the stroke is exactly know. I also verified the mass flow rate/volume flow rate from the rate of change of domain size (from initial and final volumes of domain obtained from CAD model and time) and it's correct. So the specified velocity is correct. But the mass flow rate in the simulation is very low. I checked the mass flow rate after 0.08 (total simulation time is 2 seconds) seconds and its very low as comapred to actual mass flow rate.

BTW i am using the following expression for the mesh displacement

0.0125*t

where t being the simulation time. Is "t" in CFX corresponds to simulation time? Sorry for very basic question but I just want to make sure that there is no mistake in expression.

In the domain settings under "Mesh Deformation" i am using "Displacement Rel. To = Previous Mesh" and then for moving walls under "Mesh Motion" i am using the "Specified Displacement" and specifying the displacement using the expression above. Is it correct?

In the modelling guide of CFX i read about "Mesh Motion" and "Specified Displacement" options there its written " If the Use Mesh From option is set to Initial Values, be careful with restarts because the definition of the initial mesh may have changed." Where I can find this option "Use Mesh From"? I made several restarts but didn't change anything but I think mesh is still moving correctly.

Mesh_Motion_Options.jpg

Also what's the difference between "Specified Displacement" and "Specified Location" Mesh Motion options? If I have the displacement equation (mentioned above) I should be using "Specified Displacement" right?

Sorry if i am asking a lot of questions but this is my first experience with moving mesh simulations and i am still in the learning process.

[ghorrocks]

As you are new to moving mesh I would suggest you do a simpler model first to get started. As you know the motion of the actuator, that means you know the flow rate it generates. So remove the actuator and the moving mesh and replace it with an outlet with a mass flow rate from the actuator. This is a simple steady state inlet/outlet simulation with no moving mesh and should be quite easy to do. You should also be able to get this quite accurate relatively easily, so will give you a good starting point to work from.

Once you have this simple model working well then try the more ambitious moving mesh version. As you develop the moving mesh you will then be able to compare against the simple model to check the results are reasonable.

[cfd seeker]

Originally Posted by ghorrocks

As you are new to moving mesh I would suggest you do a simpler model first to get started. As you know the motion of the actuator, that means you know the flow rate it generates. So remove the actuator and the moving mesh and replace it with an outlet with a mass flow rate from the actuator. This is a simple steady state inlet/outlet simulation with no moving mesh and should be quite easy to do. You should also be able to get this quite accurate relatively easily, so will give you a good starting point to work from.

Once you have this simple model working well then try the more ambitious moving mesh version. As you develop the moving mesh you will then be able to compare against the simple model to check the results are reasonable.

thanks for your reply. Actually i already did so, i created an outlet and using total pressure and mass flow rate B.C i did the simulation and it was quite simple. Convergence was very good and i was able to see the pressure losses and they made sense also. Now i am upto more ambitious moving mesh version

Can you please clarify my confusions from the last post?

[ghorrocks]

Specified location and Specified displacement: Let's say you have a mesh at x=1m and you want it to move right 0.1m at 1m/s. This can be defined by:

Specified Displacement = 0.1[m]*t

or

Specified Location = 1.0[m] + 0.1[m]*t

So the difference is whether it is the displacement from the initial position or the absolute position.

Check how much your mesh has moved to check it moved the distance you intended.

[Lance]

Originally Posted by ghorrocks

Specified Location = 1.0[m] + 0.1[m]*t
So the difference is whether it is the displacement from the initial position or the absolute position.

Since the the above expression will resolve into a single value, all points on that surface will collapse to that location. Probably not what you want.

Originally Posted by ghorrocks

Specified Displacement = 0.1[m]*t

This also resolves into a single value, but all points on the surface will be displaced by that value. Probably what you want.

[cfd seeker]

Thanks Glenn and Lance,

i understood the difference but the units of following expression is confusing me

Specified Displacement = 0.1[m]*t

You said if we want the mesh to move right by 0.1m. So in the above expresion Displacement = Displacement*time? "t" in above xpression do-not have units of time i.e seconds?

When you say if we want the mesh to move right by 0.1m with 1m/s. Then the expression shouldn't be Displacement = Velocity*Time?

Specified Displacement = 1[m/s]*t

Can any of you guys please clarify this?

[Lance]

Well, since displacement is a length that is obviously a typo.