# How to Monitor Mass flow rate in CFX

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 September 12, 2007, 12:46 How to Monitor Mass flow rate in CFX #1 Md Hamidur Guest   Posts: n/a 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?

 September 12, 2007, 13:23 Re: How to Monitor Mass flow rate in CFX #2 Robin Guest   Posts: n/a 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

 September 12, 2007, 14:14 Re: How to Monitor Mass flow rate in CFX #3 Md Hamidur Guest   Posts: n/a 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.

 September 12, 2007, 15:00 Re: How to Monitor Mass flow rate in CFX #4 opaque Guest   Posts: n/a 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 amirhnp, Hakuna_lee and drajkumr94 like this.

 September 13, 2007, 14:59 Re: How to Monitor Mass flow rate in CFX #5 HekLer Guest   Posts: n/a 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 Andy Von and Hakuna_lee like this.

 September 13, 2007, 15:25 Re: How to Monitor Mass flow rate in CFX #6 Hamidur Rahman Guest   Posts: n/a 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

 September 14, 2007, 10:08 Re: How to Monitor Mass flow rate in CFX #7 Dothan Guest   Posts: n/a 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

 September 14, 2007, 11:50 Re: How to Monitor Mass flow rate in CFX #8 Robin Guest   Posts: n/a 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 A_Prakash and ibadullah safdar like this.

 July 14, 2015, 08:55 #9 New Member   denizcan alaca Join Date: Jun 2015 Posts: 4 Rep Power: 9 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 gbrajtm likes this.

 July 14, 2015, 09:12 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,260 Rep Power: 136 You have to set a monitor point equal to the CEL expression for it to be visible in the solver manager.

 July 15, 2015, 03:45 #11 New Member   denizcan alaca Join Date: Jun 2015 Posts: 4 Rep Power: 9 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?

 July 15, 2015, 04:01 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,260 Rep Power: 136 You define monitor points in CFX-Pre, before you run the simulation. It is on the output tab. fatwaazam likes this.

 July 15, 2015, 06:39 #13 New Member   denizcan alaca Join Date: Jun 2015 Posts: 4 Rep Power: 9 Thanks for your help. It works as you said.

 November 6, 2015, 23:34 #14 New Member   Andy Von Join Date: Jun 2013 Posts: 3 Rep Power: 11 Thanks a lot. You really helped me.

 August 23, 2016, 12:29 #15 Senior Member   Have a nice time! Join Date: Feb 2016 Location: mech.eng.ahmedmansour@gmail.com Posts: 291 Rep Power: 9 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

 August 23, 2016, 21:14 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,260 Rep Power: 136 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.

 August 23, 2016, 21:16 #17 Senior Member   Have a nice time! Join Date: Feb 2016 Location: mech.eng.ahmedmansour@gmail.com Posts: 291 Rep Power: 9 And where can I find the solver manager?

June 22, 2017, 03:25
#18
Member

Dr Gurubasavaraju
Join Date: Dec 2014
Location: Bengaluru India
Posts: 77
Rep Power: 10
Quote:
 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.
Attached Images
 time step.PNG (9.5 KB, 55 views)

 June 22, 2017, 03:40 #19 Senior Member   urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 365 Rep Power: 10 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.

June 22, 2017, 03:51
#20
Member

Dr Gurubasavaraju
Join Date: Dec 2014
Location: Bengaluru India
Posts: 77
Rep Power: 10
Quote:
 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.

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post beguxa FLUENT 5 December 2, 2018 22:02 bcheruk CFX 15 July 6, 2017 07:30 suihenry CFX 12 May 14, 2009 18:59 Masood FLUENT 0 May 22, 2005 01:32 Paul FLUENT 9 March 23, 2002 09:37

All times are GMT -4. The time now is 00:23.

 Contact Us - CFD Online - Privacy Statement - Top