Moving PIPE
 

Hello everyone,
I have to make a moving pipe into fluid domain. Can anyone help how to model
this problem. Do you have any tutorials which will help to make this problem?
Visualisation of this problem is on attachment.
Best regards

Why are you modelling the pipe? This sounds like a simple moving mesh simulation.

I need to simulate heat transfer on moving pipe . I must make boolean operation (substract) on fluid domain to make interfaces between pipe and fluid domain ??On the sources I define a move of the pipe ? This is my first time to simulite moving parts in cfx. Earlier I only simulate immersed solid
Have You any tutorials or any links for similar simulations ?
Best regards

CFX comes with a number of tutorial examples on moving mesh.

In this case I would start with just a moving mesh simulation of the fluid domain to get that motion working and the flow correct. Once that is working then add the solid domain and its motion.

Note that this simulation will only work on CFX V15. You need to have motion in a solid to do this and V15 was the first version to support this.

hello Glen
Can You give me a title of moving mesh tutorial which I could start first
Sorry for my poor english
Best regards

"Modeling a Ball Check Valve using Mesh Deformation and the CFX Rigid Body Solver"
"Oscillating Plate with Two-Way Fluid-Structure Interaction"
"Modeling a Gear Pump using an Immersed Solid" (This one is actually immersed solids but is very useful to know as an alternate approach)
"Modeling a Buoy using the CFX Rigid Body Solver"

Hello Glenn,
I have another question for this problem.
This tutorials which You wrote on the last post are for immersed moving parts.
All these parts on t = 0 s are on the fluid. On my problem on t= 0 s pipe haven't got any connection with fluid. I define velocity on pipe 0.2 m/s and on the next delta t pipe going into fluid. How to define connections between these two domains?
I need to make cooling process for this moving pipe on the fluid domain.
Do i must make a boolean operation on fluid domain (substract area equal of pipe diameter)?
Best regards

Incorrect. The only one which uses immersed solids is the third (as I mentioned in the post). The other 3 use mesh motion. These tutorials will give you an introduction of how to do it.

I know Glenn,
I wanted to say that on the all of these tutorials on time (for example) t = 0 s or on initial boundary conditions (steady state) all moving parts are on fluid domain.
In my case pipe on time t = 0 s hasn't got any contact with fluid domain.
Best regards

When the tube advances into the domain does it stop somewhere or does it go until it hits the other wall?

Pipe passes through the entire domain . There are no collision on pipe way.

Your image shows a wall which the pipe will hit eventually. Does the pipe pass through this wall? Or is the far wall a long way away? Can you post some images of what you expect the pipe to do.

This is important as it will affect the way you model this.

I post below explanation of my problem

OK, thanks for the clarification. The way to model this is obvious now. Have a look at the quick drawing I have done.

Put the tube in a solid domain (domain 1). Put the tube inside a long cylinder, long enough to enclose the entire motion of the tube (this is domain 2). And cut a tube out of the box for domain 2 to slide through (this is domain 3).

Domain 3 is a fluid domain, stationary mesh with a transient rotor stator GGI interface. Domain 2 is a fluid domain, moving mesh with a TRS GGI to domain 3 and a static solid/fluid GGI to domain 1. Domain 3 is a moving mesh solid domain with a static solid/fluid GGI to domain 2.

Then move the mesh of domain 2 and 3 to generate the translational motion of the tube.

pipe is empty inside. This is not a tube, this is a pipe
will there be a difference if this is a pipe ??
Below is a schematic cross section of pipe .

That does not change anything. Just means the solid domain is a tube and the translating fluid domain (2) has a bit which includes the inside of the tube.

Thanks a lot Glenn,
I try your method and reply ASAP
Best regards from Poland

Hello Glenn
Can You describe in more detail ?
Best regards

Which bit don't you understand?

1 ) on frame change/mixing model (on interface) i choose option transient rotor stator.?
2) domain 2 (on Your drawing) is moving domain ?
3) domain 1 and 3 are stationary domains?
4) solid domain have a defined solid motion on solid models option?
5) which domains have turn on mesh deformation?
6) on the interface (on fluid domain) which options i need to define ??
Best regards

1) Yes, the sliding interface is transient rotor stator.
2, 3) 1 and 2 are moving mesh domains (but stationary frame of reference). 3 is a stationary frame of reference with no moving mesh.
4) No, do not select any solid motion options. Use moving mesh on a solid domain. Do not use a rigid body model.
5) 1 and 2 have mesh deformation on.
6) interface 1 to 2 is stationary I think, if that does not work then TRS. 2 to 3 is TRS.

I have another question
Where do I finf frame of reference option ?
Best regards

Frame of reference is where you choose either stationary or rotating. The default is stationary so leave it at the default for all domains.

Hello Glenn,
So I make simulation with idea which You wrote on the lasts posts and I have another problem.
On the solver only six steps go on and on the seventh error jump in with information
cNWDIST
At least one highly skewed element has been detected on a wall boundary, leading to unreliable near-wall distance calculation for the turbulent wall functions. The solver will continue to execute, but convergence and/or accuracy may be affected. Please consider improving the mesh quality. the coordinates of the element face are...
So what can I do at that moment to fix this error ??
Best regards

This tells me you have got the mesh motion wrong.

Re-run the simulation saving a results file on each time step which includes the mesh. Then have a look at the time step before it crashes at the location it specifies. If you cannot work out what the problem is post an image of it on the forum.

I increase mesh quality and simulation goes on to the 14th step.
and crashes with element volume error.
The strangest thing is that. On the 14th step and other steps before I haven't got heat transfer on the tube (on moving area of the tube).
When I define moving interface on domain 2, i need to define wall velocity ??
Best regards

The error has nothing to do with mesh quality. Have you done what I recommend in my last post?

The error is most probably due to the mesh motion settings you are using. You need to define a displacement function (versus time) and apply that to all the boundaries of the moving domain. If you miss a boundary you can get the error you got - and that includes interface boundaries so I bet you missed one of them.

So on the attachments I'm sending You what i define on interfaces of domains
Best regards

I cannot tell much about what is happening from the screen dumps. Please your CCL.

But even more important is the post I put up #25 about how to debug this. It should allow you to identify exactly what the problem is.

can You verify my defined interfaces which I send on the last post (attachments )
Best regards

I said:

The next sentence meant to say: Please attach your CCL.

But even better: if you do the images I said in post #25 I think we will be able to identify the problem straight away.

I'm sending a ccl of the simulation
Best regards

I change mesh deformation to initial boudaries on subdomain option
Then 13 steps go on and on the 14th pop up an error (attachment)
Best regards

As I thought - you have not defined the mesh motion parameters on many boundary surfaces on mesh movement domains.

Boundaries which need it are:
kostka subdom Side 2
subdomena Default

Also the Walek domain (which appears to be your solid) looks like it has no mesh deformation. You need to use mesh deformation on this domain as well.

Hello Glenn,
Thanks for reply
Where can I change on solid domain mesh deformation ??
I dont see this option on solid domain (attachment)
Best regards

What version of CFX are you using?

v15
And I have another question.
On Your schematic which domain is moving 1 or 2 ??

1 and 2 are stationary frame of reference, moving mesh domains.

OK, good. V15 is the only version which supports motion in solid domains. I am pretty sure you can do moving mesh on solid domains. You might need to edit the CCL to do this, rather than doing it in CFX-Pre. Copy the format used in your moving mesh fluid domain.

So for the first time solution goes on.
And I have interesting results.
Interface between walek and subdomain go on the direction which I defined in mesh motion but solid domain on the end of simulation is on the start position. Only interfaces walek-subdomena with empty area inside goes on.
I dont know what to define mesh deformation on solid. ccl copy paste from fluid domain doesnt work. What can I do ??
Best regards

Actually, you might need to use the solid motion options for the solid domain. Have you tried that?