CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   How to Monitor Mass flow rate in CFX (https://www.cfd-online.com/Forums/cfx/24529-how-monitor-mass-flow-rate-cfx.html)

Md Hamidur September 12, 2007 11:46

How to Monitor Mass flow rate in CFX
 
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?

Robin September 12, 2007 12:23

Re: How to Monitor Mass flow rate in CFX
 
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

Md Hamidur September 12, 2007 13:14

Re: How to Monitor Mass flow rate in CFX
 
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.

opaque September 12, 2007 14:00

Re: How to Monitor Mass flow rate in 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


HekLer September 13, 2007 13:59

Re: How to Monitor Mass flow rate in CFX
 
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


Hamidur Rahman September 13, 2007 14:25

Re: How to Monitor Mass flow rate in CFX
 
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

Dothan September 14, 2007 09:08

Re: How to Monitor Mass flow rate in CFX
 
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

Robin September 14, 2007 10:50

Re: How to Monitor Mass flow rate in CFX
 
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 July 14, 2015 07:55

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 July 14, 2015 08:12

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

denizcan alaca July 15, 2015 02:45

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 July 15, 2015 03:01

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

denizcan alaca July 15, 2015 05:39

Thanks for your help. It works as you said.

Andy Von November 6, 2015 23:34

Thanks a lot. You really helped me.

Ahmed Saeed Mansour August 23, 2016 11:29

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 August 23, 2016 20:14

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 August 23, 2016 20:16

And where can I find the solver manager?

gbrajtm June 22, 2017 02:25

1 Attachment(s)
Quote:

Originally Posted by denizcan alaca (Post 555394)
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 June 22, 2017 02:40

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 June 22, 2017 02:51

Quote:

Originally Posted by urosgrivc (Post 654403)
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.

urosgrivc June 22, 2017 03:09

and why is the 1st solution I mentioned not ok?

Just load your 15th timestep or choose from the (clock) tipe of buton on top in post

gbrajtm June 22, 2017 03:57

2 Attachment(s)
Quote:

Originally Posted by urosgrivc (Post 654409)
and why is the 1st solution I mentioned not ok?

Just load your 15th timestep or choose from the (clock) tipe of buton on top in post

My requirement needs a force from expression.

I am using this expression in optimisation problem as the output parameter to design of experiments (DOE). This DOE takes the values of the first time step, which not a desirable for my problem. Instead, i want maximum value of force among all time steps (nearly 250 are there in my analysis).
To obtain this I have to write an expression which could calculate the force at a particular time (time belong to max value of force) then i can assign this expression as the output parameter to DOE.

urosgrivc June 22, 2017 07:06

Now this is quite a diferent thing than originaly posted.
i think this will be a tough nut to crack.

I am thinking something about; if and acumulated timestep but i doubt that this will work in this case,

gbrajtm June 22, 2017 08:28

Yea, I am trying all possible ways but it still taking the default time. If could manage to calculate the force though CEL with a current time step, it would solve my problem. Since I know which time have maximum value of Force.

Thank you.


All times are GMT -4. The time now is 15:21.