[stfahim]

Hi, I am working with a steam generator and a pump which are connected to a reactor. I want to set the pressure loss/drop in both of them. Additionally, for steam generator I want to add a negative heat transfer per unit volume. But I couldn't find any exact tutorial for that. Can anyone help?

[ghorrocks]

One approach is to use a momentum source term for the pump and pressure loss through devices, and to use a heat source term for the steam generator.

Alternately you can model that actual devices to generate the pressure/heat gains/losses.

[stfahim]

Can you tell me specifically where are these options of adding a momentum source and a heat source?
I tried to create domain and then boundary but unfortunately I couldn't find these extra options.

[ghorrocks]

You can add source terms three ways:

As a source point (then it acts at the element you apply it to)
On a boundary face (then it acts on the boundary face you apply it to)
Or on a volume (then it acts on the volume).

Source point is a stand-alone option. Boundary face is one of the tabs in the boundary condition tab. For a volume source, you need to define the volume in your mesh, then make it a sub-domain. You can then apply the source term to the sub-domain.

[stfahim]

Thank you for your help. 😄

[stfahim]

If I want to do a mesh independence test in cfx what is the procedure? I didn't find any suitable tutorial on it. I know this only for fluent.

[Gert-Jan]

Why not use the procedure for Fluent? Should not differ much, I would guess.

[stfahim]

Can you guys tell why this is appearing and how to solve this?

[ghorrocks]

You should deal with errors one at a time, with the first reported error being the key one.

In this case you are getting a bounds error. So change the table range to cover the temperature and pressure range in your simulation, with a bit of tolerance added for numerical convergence.

The later errors are probably caused by this one, so fix the bounds error first.

[stfahim]

What is meant by the table range?
actually there are a lot of parameters in the setup; so it is a bit difficult for me to understand.

[ghorrocks]

(I am not at work at the moment so cannot get the exact page up - but it is something like this):
In the materials setup on the properties table expand out the options and you will see settings for the table generation. What this does is CFX takes your material model and evaluates the material properties at the points defined in the table, then during the simulation it uses the table rather than your function. This is why you need to make sure the table is appropriately sized for your simulation as it needs to be big enough to cover the range of interest, but not so big that you loose detail.

[stfahim]

I want to assign pressure drop as a function of flow rate. I created a table based on the values of the flow rate and its corresponding pressure values and defined a user function. Then I created an expression named pd(volume flowrate) but it doesn't work. What is the correct expression for the flow rate in the bracket?

Do the expression name and the user function name have to be the same?

[ghorrocks]

What type of user function did you use? Interpolation? CEL? User fortran?

[stfahim]

I changed the user function a little bit. I gave values of velocity now (m/s) instead of flow rate and its corresponding pressure values(kg m^-2). Then I created the table and completed the user function. I assigned it a name "PD".
Then in the expression I defined it as PD(Velocity) with name pd. And it shows the exact graph in the plot option.
But when I try to enter this expression in the required section(pump pressure change) an error is shown. I have attached the photos. It is saying expected units in kg m^-1 s^-2. But I don't know how to solve this issue.

[Opaque]

Your "Results Units" in the interpolation function are incompatible with Pressure units.

I guess they are in [Pa] or some multiple of them.

[stfahim]

How to solve this? I am a newbie in case of matching units.

[Opaque]

Check how you defined the interpolation function.

Once you correct the definition/creation of the interpolation function, your units should be compatible. I cannot tell you what to change since I do not know the source of the data used to define the CEL function.

I also forgot to mention that after you fix your units, you should modify the usage of the function from

PD(Velocity) to either PD (Velocity u/v/w) or PD(MyNormalVelocity)

The expressions in CFX Solver do not support Velocity (vector) as an input for a required scalar, i.e. you must provide a scalar (say velocity component or velocity projection)

[stfahim]

If I want to get a reverse flow should I have to write PD(-u)? Assuming the velocity in -ve x direction. Or it should be -PD(u)?

[stfahim]

Thank you guys. I was able to match the units and get the desired results. Though I didn't use the table as the average velocity in this case was not easy to calculate. So I created an equation and it worked with good precision.

[stfahim]

I have some additional questions. Please answer if you can.
1. If I get my desired results without setting any convergence criteria within cfx, and the results are 1-5% (one flow rate) and 8%(three other flow rates) of the design parameters, do I need to do a mesh sensitivity test? As the user points(flow rates and temperatures) are more or less constant.
2. Also, if I set a convergence criteria and the solution doesn't converge within the set iteration number but if I see the results are more or less constant then can I conclude that my solution is converged? In that case, should I need to do a mesh sensitivity test?