Hi, I am simulting flow over a axial gas turbine blade with 30 stator blade and 60 rotor blade. I want to see convergence of mass flow rate at a perticular point in the domain. I know this could be done from user monitor option. But mass flow rate option is not available. Could anyone please tell me how to do that?

Hi Hamidur,

Mass Flow cannot be calculated at a point, you need a surface through which to define the mass flow. The residuals tell you the imbalance, but CFX only reports the Maximum (MAX) and Root Mean Square (RMS) residual. I don't think you can output the residual at a point.

What exactly is your concern? If you are concerned about the imbalance of mass, this is calculated as the mass into the domain minus the mass out of the domain and is reported to the monitor file already, you just need to plot it.

Regards, Robin

Thanks for your comments. Actually I need to plot Mass flow rate against the iteration. This plot is possible in fluent but I am not sure about CFX.

Dear Md Hamidur,

You are not being specific on which Mass Flow Rate you want? Do you want the mass flow rate on the inlet, outlet, a 2d region within the domain?

If you know which 2d region you want, you can monitor it by creating a Output Control/Monitor Points. Select the option Expression and type somethin along the lines of

Expression = massflow()@YourInlet

Expression = massflow()@TheOutlet

Expression = massflow()@REGION: some defined region

Hope it helps,

Opaque

This can be done in CFX, just as easy as Fluent.

In addition to opaque's comments, which require you to create a monitor point in CFX Pre, you do not need to do this if you want to monitor the mass flow rate through an existing boundary condition (eg: inlet, outlet, interface boundary, etc..):

- Create a new montior in the solver manager and call it something, say "My Mass Flow Monitor"

- Pick "FLOW" in the tree

- Pick the domain name you want and then the boundary you want

- Monitor the "P-Mass" flow through that boundary

Thank you guys. I did it succesfully. One more problem that I have been experiencing now and that is "wall has been placed at the outlet boundary". I know that it means there is a reverse flow at the exit of the domain. Is there any way to get rid of this instead of playing with the boundary condition? Thanks to you all

Hi, I think the only method is to move the surface where you define the BC, il the problem is well posed.

I belive that wall placed by CFX can help the convergence for the initial iterations but if the convergence is reached with this notice, the solution is totally unphysic.

Remain to understand if this notice disapper, is the final solution affected by the convergence story?

Dothan

Hi Hamidur,

It depends on what's going on at the outlet. You should try and match the physical conditions as closely as possible. If there is likely to be separation and recirculation near the outlet and this is a region of interest, you should move your outlet further downstream to resolve the necessary flow features. If your outlet is far from the region of interest, you can probably ignore the warning.

Before you modify your geometry, consider trying some of the other options for the outlet mass flow specification. By default the solver will scale the local flow rate at the outlet to allow a natural pressure profile to develop. Other options are to set the mass flow to "Constant Flux" and "Scale Pressure".

Constant Flux will enforce a uniform mass flux across the surface. This is what most codes do at a mass flow outlet, but may be unphysical. It is useful for bleeds or outlets where you just want to pull the mass out and aren't concerned about the profile and is usually more stable.

Scale Pressure requires that you enter a pressure profile (by CEL), which the solver will shift up and down in order to get the appropriate mass flow rate. A very common way to use this is to simply specify a constant value for the pressure profile (any constant value will do), in which case the boundary condition will have a constant static pressure across the face. This is physically realistic if your outlet ejects into a larger domain or plenum.

Regards, Robin

[denizcan alaca]

I am not sure whether you are still in forum after 8 years but i am going to take my chance and revive the topic

What if i want to monitor pressure drop or area average pressure on a stated surface. I specified a CEL expression for total pressure on inlet and outlet then i specified another CEL for areaAve(Total Pressure)@inlet-areaAve(Total Pressure)@outlet which defines pressure drop through inlet to outlet. I check monitor properties to add pressure drop plot to see how it changing with unbalanced RMS but i could not find it.

Regards
Denizcan

[ghorrocks]

You have to set a monitor point equal to the CEL expression for it to be visible in the solver manager.

[denizcan alaca]

Can you clarify please?
For example I have expression that is named as 'itp'. Then in Solver Manager, I click new monitor and set new monitor's name as 'itp' but it is not visible as you said. Am I doing something wrong?

[ghorrocks]

You define monitor points in CFX-Pre, before you run the simulation. It is on the output tab.

[denizcan alaca]

Thanks for your help. It works as you said.

[Andy Von]

Thanks a lot. You really helped me.

[Ahmed Saeed Mansour]

Where can I find the file of the results of the monitor...when I set it in fluent I can generate a txt file...I need this in cfx..please

[ghorrocks]

Define a monitor point with it, then it will be accessible in solver manager. You can export the raw data from the solver manager if you like.

[Ahmed Saeed Mansour]

And where can I find the solver manager?

[gbrajtm]

Originally Posted by denizcan alaca

I am not sure whether you are still in forum after 8 years but i am going to take my chance and revive the topic

What if i want to monitor pressure drop or area average pressure on a stated surface. I specified a CEL expression for total pressure on inlet and outlet then i specified another CEL for areaAve(Total Pressure)@inlet-areaAve(Total Pressure)@outlet which defines pressure drop through inlet to outlet. I check monitor properties to add pressure drop plot to see how it changing with unbalanced RMS but i could not find it.

Regards
Denizcan

Hello,

I wanted to calculate the force for a particular time in transient analysis, what modification I have to do for this CEL (force_x()@piston)?
At present I am selecting each time step to calculate force, instead, i want the force to calculated for particular time using the expression.
Please let me know if any other alternatives.
Thanks in advances

[urosgrivc]

And you already have the resuls or what?

1: If you do than in cfx post you can click on calculators=>function calculator=>(force,area,direction)
And you will get your force for an active (curently opened) timestep.

2: You can make a chart from this same expression and look at that 15th value.

[gbrajtm]

Originally Posted by urosgrivc

And you already have the resuls or what?

1: If you do than in cfx post you can click on calculators=>function calculator=>(force,area,direction)
And you will get your force for an active (curently opened) timestep.

2: You can make a chart from this same expression and look at that 15th value.

I have results already, I am doing same as you mentioned. But my requirement is I wanted to calculate force for that particular @ area and @ time using an expression. I went through all tutorial but failed to find a solution.