[JM27]

Hi there, I am hoping to get some help on 2d axisymmetric simulation in ccm+. Been stuck on this for a few days now so any suggestions would be appreciated...

I am trying to run a 2d axisymmetric simulation with moving boundary using the mesh morpher solver. My set up involves a square domain with the right boundary set as the axis of symmetry. The top boundary is a pressure outlet at 100kPa and 300K (also initial conditions). The lhs boundary is a stationary wall (fixed boundary plane specification) and the bottom wall (radial axis) is moving according to a grid velocity.

I specify the grid velocity using a field function x(r,t) - which is a combination of an exponential function and a cosine. The grid velocity therefore changes as a function of time and radial position r.

I generate a trimmed cell mesh with prism layers on the moving boundary to capture the high gradients in this region. The models that I am using are:

Axisymmetric, Gradients, IF97 Water (compressible), implicit unsteady, laminar, segregated flow, and segregated fluid temperature.

Here goes my problem:

I initialize the problem and so far all looks good (or as I think it should). Upon trying to step the simulation, the following error comes up:

Non-zero radial coordinate found on axis boundary rhs

Maximum error was :0
Repair boundary using "Project to Axis...".
Command: StepSimulation
error: Server Error

I am surprised by this since I set up the domain/mesh as described in the user-guide for axisymmetric meshes, i.e. i) in Z=0 plane ii) with the axis of symmetry on the x-axis iii) mesh above y=0.

Anyway, I have tried using Project Axis but it still does not work. Instead, a floating point error comes up:

A floating point exception has occurred: floating point exception [Invalid operation]. The specific cause cannot be identified. Please refer to the troubleshooting section of the User's Guide.
Command: Unknown Command
error: Server Error

I think that the problem lies in my field function for the Grid Velocity. I have tried running the exact same thing but with a constant velocity i.e. I specify a constant value directly rather than as a function of exp and cos and it works. I have tried increasing the complexity of the function step by step by introducing the cos and exp function separately. The cos function works but not the exp.

An interesting thing I noticed is that the exponential function contains the dependence on the radial coordinate r i.e. e^br where b is a constant. cos is expressed in terms of time.


Please help.... I do not think this should be that difficult to set up and run

[Ubuntu]

Originally Posted by JM27

I am trying to run a 2d axisymmetric simulation with moving boundary using the mesh morpher solver. My set up involves a square domain with the right boundary set as the axis of symmetry. The top boundary is a pressure outlet at 100kPa and 300K (also initial conditions). The lhs boundary is a stationary wall (fixed boundary plane specification) and the bottom wall (radial axis) is moving according to a grid velocity.

I specify the grid velocity using a field function x(r,t) - which is a combination of an exponential function and a cosine. The grid velocity therefore changes as a function of time and radial position r.

Will your domain look like a nozzle with variable area inlet in 3D?

[JM27]

Hi Ubuntu,



No it will not have a variable area inlet in 3D...I am trying to model an ultrasonic cleaning tank.



I want the boundary motion in my simulation to account for the acoustic wave in the tank filled with water...So if I revolve my axisymmetric geometry to get 3D this would look just like a cylinder (or pipe) but with one end closed (moving wall) and the other end open to atmosphere (pressure outlet)...hope this clarifies

[Ubuntu]

Does the attachment look like what you wanted? more or less?

https://we.tl/t-9YMy02OVyQ

I had some free time.

[JM27]

Hello again Ubuntu,

Thanks for your reply. Yes looks close enough to what I am trying to do.

The main difference I notice is that in the attached video the oscillation seems to be varying only with time. In my case I need the oscillation to also be varying with position..mainly because I want the motion at the left wall (r=0.06m) to be fixed and the maximum motion to take place at the axis of symmetry (r=0).. in fact that is why i am using an exponential function of the form exp^(-br) in my field function...r is the radial position and b is a constant.
At r = 0 the mesh displacement would be maximum and minimum at r=0.06m (left boundary) the mesh displacement would be zero.

Can you explain how you did your simulation in CCM+ and any suggestions for my case?

That would be very helpful for me, thanks in advance!

[Ubuntu]

Originally Posted by JM27

Can you explain how you did your simulation in CCM+ and any suggestions for my case?

Sure, happy to.

I used the same boundary conditions as you described in your post (see attachment) except that I used laminar, without energy equation terms.

Originally Posted by JM27

Non-zero radial coordinate found on axis boundary rhs

In my case, the axis boundary was along the X-axis, and the mesh was on the XY plane above y =0. I am not sure why it happens to you though you followed all these.

Regarding the morphing motion, I created a simple Field Function which looks like,
sin(2*$Time)
In your case, it will be like
exp(-$$Position[1])*sin(2*$Time)
The location of lab coordinate system is important when you use $$Position[].

Hope this helps you.

[JM27]

Originally Posted by Ubuntu

Sure, happy to.

I really appreciate you trying to help out!

Originally Posted by Ubuntu

I used the same boundary conditions as you described in your post (see attachment) except that I used laminar, without energy equation terms.

I am also using laminar However, ccm+ won't let me run without specifying an energy model. I tried both Segregated Fluid Isothermal and Segregated Fluid Temperature and it still does not work

Originally Posted by Ubuntu

In my case, the axis boundary was along the X-axis, and the mesh was on the XY plane above y =0. I am not sure why it happens to you though you followed all these.

With regards to this problem, I have created a new geometry part (again based on the conditions for axisymmetric model) and regenerated a new mesh and this error no longer comes up

Originally Posted by Ubuntu

Regarding the morphing motion, I created a simple Field Function which looks like,
sin(2*$Time)
In your case, it will be like
exp(-$$Position[1])*sin(2*$Time)
The location of lab coordinate system is important when you use $$Position[].

Hope this helps you.

If you don't mind have a few questions about the morphing itself. It would be really helpful if you could answer these so I can cross-check my simulation setup with yours. I am using the following field function to specify Grid Velocity:

[((($$Position[1] <= 0.06) && ($$Position[0] <= 3e-4) ) ? (( (2*3.1416*33e3)*(0.2e-6) * (cos(2*3.1416*33e3*${Time}))*(exp(pow(-(-2e8)*$$Position[1],6))))) : 0 ),0,0]

I have also tried replacing $$Position[1] with $RadialCoordinate but still won't work. It does work if I get rid of the exp(pow(-(-2e8)*$$Position[1],6)) bit however

1) In your field function, do you use some kind of condition or do you specify the velocity as a vector directly, i.e. [x,y,z] components?
2) What mesh morpher solver conditions are you using? In my case, I'm using Morph from Zero and Recompute Interfaces
3) I was using a Fixed Boundary Plane Specification on my left boundary. I tried it using Floating as in your case but I keep getting this error:

SIGSEGV: memory access exception Command: StepSimulation
Processor: 0
Recoverability: Non-recoverable
ServerStack: [
libStarNeo.so: SignalHandler::signalHandlerFunction(int, siginfo*, void*),
libpthread.so.0(+0xf6d0),
libMorpherModel.so(+0x1534d6),
libMorpherModel.so(+0x1591ce),
libMorpherModel.so(+0x159af6),
libMorpherModel.so: ProMorpher::update(int const&, double const&),
libMorpherModel.so: ProMorpherMap::run(int, double),
libMorpherModel.so: MovingMeshSolverBase::updateThisTimeStep(FvReprese ntation const&),
libMorpherModel.so: MovingMeshSolverBase::commonTimeStepUpdate(unsigne d int const&),
libStarSolve.so: ImplicitUnsteadySolver:: preStep(),
libStarSolve.so: ImplicitUnsteadySolver::step(),
libStarSolve.so: SimulationIterator::startSimulation(RunnableSolver *, int, SimulationIterator::RunMode, bool),
libStarSolve.so(+0x1e6357),
libStarNeo.so: Controller::executeCommand(Command&, Properties const&, Properties&),
libStarNeo.so: Controller:: processCommands(),
libStarMachine.so: CommandController::SerialMasterCommandLoop::start( ),
libStarMachine.so: CommandController:: processCommands(),
libStarMachine.so: Machine::startServerHost(int, char**, std::map<std::string, unsigned int, std::less<std::string>, std::allocator<std: pair<std::string const, unsigned int> > >&),
libStarMachine.so: Machine::main(int, char**)]
Signal: SIGSEGV: memory access exception
error: Server Error

I am running on 16GB ram so again surprised to have this come up. I am running out of ideas to try make this work
Your help is very much appreciated, at least I know I am on the right track Look forward to your reply!

[Ubuntu]

Originally Posted by JM27

1) In your field function, do you use some kind of condition or do you specify the velocity as a vector directly, i.e. [x,y,z] components?
2) What mesh morpher solver conditions are you using? In my case, I'm using Morph from Zero and Recompute Interfaces
3) I was using a Fixed Boundary Plane Specification on my left boundary. I tried it using Floating as in your case but I keep getting this error:

1. I didn't make it as a vector function. You can specify it as components so that you don't have to create a vector field function (Fig1 and 2)
2. I didn't change any solver settings of morpher (default). I went to respective boundaries and specified morpher conditions for each of them.
3. I am not sure why.

What is the equation you wish to put as field function? I wonder if that conditional statement in your field function is really necessary. May be placing a new coordinate system will help, I think.
Also I made some changes in the field function (Fig3) and did it again.
Check if this looks more like what you want.
https://we.tl/t-Vvft7y2mOc

[JM27]

Hello again Ubuntu,

Thank for your reply and apologies for the delay in reply

Originally Posted by Ubuntu

1. I didn't make it as a vector function. You can specify it as components so that you don't have to create a vector field function (Fig1 and 2)

I have eliminated the use of the condition in my field function and just specified the components and it works okay. I think the condition is just an extra complication in this case...

Originally Posted by Ubuntu

2. I didn't change any solver settings of morpher (default). I went to respective boundaries and specified morpher conditions for each of them.

Ok, just wanted to double check

Originally Posted by Ubuntu

3. I am not sure why.

What is the equation you wish to put as field function? I wonder if that conditional statement in your field function is really necessary. May be placing a new coordinate system will help, I think.
Also I made some changes in the field function (Fig3) and did it again.
Check if this looks more like what you want.
https://we.tl/t-Vvft7y2mOc

Yes, this is more similar because motion at the side wall is fixed.
The equation I am using is of the form: const*exp(const*$$Position)*cos(const*${Time})

After lots of trial and error I figured that the memory access exception error was in fact coming from the field function. I eliminated the condition and declared the two functions, i.e. trigonometric and exponential, as two separate field functions. I create a third field function in which I reference the trig and exp function as vector components.

Still curious as to why it wouldn't work by simply putting the whole definition in a single field function, but I'm glad I finally managed to get the desired motion on the boundary

Hope this helps anyone having the same problem in the future. Thanks a lot Ubuntu for your help

[Ubuntu]

Glad to know that you solved it.