CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Setting a pressure loss in cfx

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 18, 2021, 15:24
Unhappy Setting a pressure loss in cfx
  #1
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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?
stfahim is offline   Reply With Quote

Old   March 18, 2021, 17:22
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,726
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 18, 2021, 19:50
Default Where are these options
  #3
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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.

Last edited by stfahim; March 18, 2021 at 19:51. Reason: Spelling mistake
stfahim is offline   Reply With Quote

Old   March 18, 2021, 23:06
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,726
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 22, 2021, 18:54
Talking Thank you
  #5
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
Thank you for your help. 😄
stfahim is offline   Reply With Quote

Old   March 31, 2021, 07:30
Default mesh independence test
  #6
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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.
stfahim is offline   Reply With Quote

Old   March 31, 2021, 07:33
Default
  #7
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,335
Rep Power: 20
Gert-Jan will become famous soon enough
Why not use the procedure for Fluent? Should not differ much, I would guess.
Gert-Jan is offline   Reply With Quote

Old   May 28, 2021, 01:04
Unhappy Stack overflow error
  #8
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
Can you guys tell why this is appearing and how to solve this?
Attached Images
File Type: jpg time step error.jpg (130.1 KB, 10 views)
File Type: jpg fatal overflow in solver.jpg (95.2 KB, 7 views)
File Type: jpg Screenshot_20210528-075038.jpg (42.1 KB, 6 views)
stfahim is offline   Reply With Quote

Old   May 28, 2021, 01:35
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,726
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   May 28, 2021, 18:33
Default table range
  #10
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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.
stfahim is offline   Reply With Quote

Old   May 29, 2021, 01:39
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,726
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
(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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 7, 2021, 11:23
Unhappy How to write volume flow rate expression
  #12
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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?
stfahim is offline   Reply With Quote

Old   June 8, 2021, 05:59
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,726
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
What type of user function did you use? Interpolation? CEL? User fortran?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 8, 2021, 09:06
Unhappy
  #14
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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.
Attached Images
File Type: jpg IMG_20210608_160112.jpg (147.8 KB, 9 views)
File Type: jpg IMG_20210608_160203.jpg (164.0 KB, 7 views)
File Type: jpg IMG_20210608_160238.jpg (162.7 KB, 6 views)
File Type: jpg IMG_20210608_160259.jpg (124.6 KB, 6 views)
stfahim is offline   Reply With Quote

Old   June 8, 2021, 09:11
Default
  #15
Senior Member
 
Join Date: Jun 2009
Posts: 1,404
Rep Power: 27
Opaque will become famous soon enough
Your "Results Units" in the interpolation function are incompatible with Pressure units.

I guess they are in [Pa] or some multiple of them.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   June 8, 2021, 09:21
Unhappy
  #16
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
How to solve this? I am a newbie in case of matching units.
stfahim is offline   Reply With Quote

Old   June 8, 2021, 09:57
Default
  #17
Senior Member
 
Join Date: Jun 2009
Posts: 1,404
Rep Power: 27
Opaque will become famous soon enough
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)
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   June 8, 2021, 11:03
Default
  #18
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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 is offline   Reply With Quote

Old   June 9, 2021, 20:30
Smile Thank you
  #19
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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 is offline   Reply With Quote

Old   June 9, 2021, 20:32
Unhappy Question about mesh sensitivity test
  #20
New Member
 
Saiyed Tasnim Md. Fahim
Join Date: Sep 2018
Location: Obninsk Institute for nuclear power engineering
Posts: 22
Rep Power: 4
stfahim is on a distinguished road
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?
stfahim is offline   Reply With Quote

Reply

Tags
cfx, negative heat transfer, pressure drop, pump, steam generator

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind tunnel Boundary Conditions in Fluent metmet FLUENT 6 October 30, 2019 12:23
Periodic flow using Cyclic - comparison with Fluent nusivares OpenFOAM Running, Solving & CFD 30 December 12, 2017 05:35
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
Warning 097- AB Siemens 6 November 15, 2004 04:41


All times are GMT -4. The time now is 11:29.