[749604]

I am trying to model a valve using CFX. It is supposed to be a simple 2D simulation and involves a region of high pressure helium entering another region of air at atmospheric pressure. The high pressure (310 bar) helium enters the air region through a 3.5 mm inlet and there is a 20 mm opening in the air region. I've assumed that the helium region is just an infinite volume at 310 bar. I have a geometry for the second region which is basically a rectangle with an inlet at the bottom and an opening on the side wall.

How should I define the inlet and outlet boundary conditions? i do not know the mass flow rate or velocity at inlet so I have set the total pressure to 310 bar with reference pressure 1 atm. The outlet of the air region is given a static pressure with 0 relative pressure.

I have seen in the documentation that it is not advised to specify pressure at both the inlet and outlet but that is the only information I have.

The outside of the outlet is also at 1 atm like the air region.
The air region has a wall around it apart from the inlet and outlet.
I am also confused as to how to model the volume of the air region, I have a value for the volume but I am doing a 2D simulation in xy plane (2 elements in z-direction) so how can i relate the 2D rectangle to the volume I need?



New mesh:

[JuPa]

Provide us with a picture.

[749604]

Added image.

[ghorrocks]

This flow is going to be high Mach number so you are going to need a better quality and resolution mesh that what you have.

It is fine to use pressure inlets and outlets if that is the information you have. They are just a little harder to converge than massflow/pressure combinations.

[Opaque]

Regarding your concern about using pressure boundary conditions, the documentation only says that such combination is sensitive to the initial guess, and as Glenn mentioned, they are little harder to converge.

Why are they sensitive to converge ? Let us use look at simple duct flow with total pressure inlet with static pressure outlet. In such configuration, we are already bounding the maximum mass flow through the system since for a flow with no losses, the difference between the total and static pressure is the dynamic head (rho*v^2 / 2 for incompressible fluid), and since the area is known the velocity is also implied. Using an initial guess above such value will be non-physical.

For the same example, the combination of static pressure inlet and static pressure outlet would be even worse since the pressure difference can only be balanced by the losses which are a function of the wall shear. Such setup may (if it does) only converge if the mesh is good enough for the flow model (laminar or turbulent) to predict the wall shear to match the pressure drop.

That is my interpretation of the recommendations,

[749604]

Thanks for the help guys. I have refined the mesh. I have an additional question, if I have one element in the extruded direction do I set symmetry boundary conditions on the top and bottom walls? Or should I just leave it as 2 or 3 elements in the extruded direction?

Here are some results, I changed the geometry a little. The first 2 images are using 3 elements in the extruded direction and the second 2 images are using 1 element in the extruded direction with symmetry boundaries on top and bottom surfaces. So there's clearly a big difference, so am i doing something wrong?

3 elements in z-direction




1 element in z-direction

[ghorrocks]

No, what you are doing is essential. What it is suggesting is that your flow is not 2D but is more likely 3D. I would recommend extruding a reasonable distance in the z direction and giving it plenty of mesh elements. Run a simulation (almost certainly transient is required) and I bet you will find it is 3D and transient.

[749604]

Ok, I have changed the geometry to make it more 3D. Evidence would suggest that the results i was getting before were indeed incorrect. My problem now is that I can't get CFX to run my new setup.

It runs for 1 complete iteration then gives me this error:

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction.
| Message:
| Floating point exception: Multiple faults
|
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction.
| Message:
| Stopped in routine FPX: C_FPX_HANDLER
|
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve:
|
| The ANSYS CFX solver exited with return code 1. No results file
| has been created.
+--------------------------------------------------------------------+

This is my mesh:

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[749604]

Ok, well i've changed the geometry again as it seems i'm going to need a more accurate model anyway.
My geometry now looks like this:


I have two domains connected at an interface, if I want the lower domain (domain 2) to be at 309 bar and domain 1 to be at atmospheric pressure do I just set that in the initialisation conditions tab?

Edit: I should be expecting velocities of around Mach 3, is CFX still suitable for simulating this?

[ghorrocks]

CFX has models appropriate to go up to around Mach 5. In other words CFX does not have hypersonics models (eg dissociation), but supersonic and transonic flow is modelled.

Then you just initialise one domain to be one pressure and the other to be another. But this does not seem to require multiple domains. Model it as one domain and use an initial condition which uses the inside function or a function of z height to define the pressure.

[749604]

I would like to have the option of changing the fluid properties of the two domains so I kept them separate. I have tried different initialisations for domain 2 whilst keeping domain 1 the same but I can't get any flow between the two domains. For instance I set the w component of velocity to 50 m/s in domain 2 to try and get flow along the +ve z-direction up into domain 1 but it doesn't instead the streamlines do this:

[ghorrocks]

I would like to have the option of changing the fluid properties of the two domains so I kept them separate.

No, bad idea. I read from your initial post that it is high pressure helium escaping into low pressure air. In this case you should be using a single domain, multicomponent simulation. This will also account for the mixing of the two gases.

[749604]

Thanks for the advice Glenn, I have the simulation working at the moment, I just needed to use a much smaller timestep. At the moment i'm just modelling pressurised air so I'm still using two domains. Is there a simple way in CFX post to produce a graph of maximum pressure in a domain against time? Or do I need to find the location of maximum pressure and just plot the pressure from that location each timestep?

[ghorrocks]

This simulation does not need two domains, regardless of what fluid model you use. It should be a single domain. But the penalty of running multiple domains is usually low, so hopefully you get away with it.

Put a monitor point in with something like maxVal(pressure)@DomainName. Then run the simulation and it will appear on the solver monitors in Solver Manager.

[749604]

Great, thanks. I am a little unsure about setting up a multicomponent flow. If I set it up as one domain where do I specify that the lower volume is at 309 bar? At the moment i'm using the domain initialisation to set up the pressure which would include the entire geometry if I only have one domain.

[ghorrocks]

Try the reacting flow in a mixing tube tutorial.

You can define initial conditions with CEL expressions, such as if(x>3[m],309[bar],0[bar]) or you could define a mesh region as a subdomain and use if(inside()@SubdomainName,309[bar],0[bar])

[749604]

Ok, so if I want to have the pressurised helium entering into atmospheric air I can't avoid using CEL expressions?

[ghorrocks]

There are many ways of doing this and they are all quite simple. Multiple domains works - but has disadvantages (reduced quality of partitioning of the domains for instance).

[749604]

Hi Glenn, I have a few of questions.

1. Does the expression "if(x>3[m],309[bar],0[bar])" require a locator? Or does it automatically apply to all domains?

2. Can a similar expression be used to define fluid properties/materials or volume fractions?

3. To initialise the if statement do I just create an expression with it in and then it will be applied by the solver?

4. I have seen in the CFX solver advanced controls that there are some options for running simulations on multiple CPU cores, is it as simple as selecting one of the local multi core options? I tried this but it doesn't seem to work.

Appreciate the help!