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

Obtaining negative pressure transients

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 7, 2020, 10:39
Default Obtaining negative pressure transients
  #1
New Member
 
John Applesmith
Join Date: Feb 2020
Posts: 13
Rep Power: 6
ns778 is on a distinguished road
Hello,

I need to obtain dp/dt in a fluid domain so for each node I'd like to obtain how much the absolute pressure changes from the last time-step. I can then divide by the time-step to get dp/dt.

Additionally, I would then like to index the maximum pressure transient over the volume at each time-step and plot the maximum obtained dp/dt against simulation time. There are moving immersed solids in my simulation if it makes a difference. I am simulating the flow across an aortic bi-leaflet valve.

Thanks.
ns778 is offline   Reply With Quote

Old   May 7, 2020, 13:42
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,815
Rep Power: 32
Opaque will become famous soon enough
In case it helps, you should be able to use (only in the solution step)

Absolute Pressure.Time Derivative

in any expression as well as the RHS of an algebraic Additional Variable.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 10, 2020, 04:04
Default
  #3
New Member
 
John Applesmith
Join Date: Feb 2020
Posts: 13
Rep Power: 6
ns778 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
In case it helps, you should be able to use (only in the solution step)

Absolute Pressure.Time Derivative

in any expression as well as the RHS of an algebraic Additional Variable.
Hi, is this a Derived Variable to be added in the workspace during a run? I can't find this function in the documentation anywhere but sounds exactly what I need.
ns778 is offline   Reply With Quote

Old   May 10, 2020, 20:25
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,815
Rep Power: 32
Opaque will become famous soon enough
What do you need to do with it? Use it in an expression? or copy it into another variable?

For an algebraic additional variable, you can do

Additional Variable Value = Absolute Pressure.Time Derivative

or use as part of any expression:

MyExpression = 2 * Absolute Pressure.Time Derivative
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 11, 2020, 02:46
Default
  #5
New Member
 
John Applesmith
Join Date: Feb 2020
Posts: 13
Rep Power: 6
ns778 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
What do you need to do with it? Use it in an expression? or copy it into another variable?

For an algebraic additional variable, you can do

Additional Variable Value = Absolute Pressure.Time Derivative

or use as part of any expression:

MyExpression = 2 * Absolute Pressure.Time Derivative
Hi, I saw your message on a similar thread years ago and just added Absolute Pressure.Time Derivative as CEL in Set-Up: many thanks.

Is it possible to access the volume-maximum of this value at each time-step? So I could plot dp/dt against t and identify when in the simulation the maximum pressure transient occurs and then where using an isosurface? I'm unsure of how to access the domain maximum of a value at a time-step and have 0 experience with Fortran or User Routines.
ns778 is offline   Reply With Quote

Old   May 11, 2020, 05:34
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Most functions in CFX can be done using CEL and do not need user fortran.

To get the maximum of this function at each timestep use the CEL expression:
maxVal(MyExpression)@Domain Name

Look in the CFX Reference manual for the other available CEL functions and expressions.
__________________
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 11, 2020, 07:30
Default
  #7
Senior Member
 
Join Date: Jun 2009
Posts: 1,815
Rep Power: 32
Opaque will become famous soon enough
What do you need to do with it? Use it in an expression? or copy it into another variable?

For an algebraic additional variable, you can do

Additional Variable Value = Absolute Pressure.Time Derivative

or use as part of any expression:

MyExpression = 2 * Absolute Pressure.Time Derivative
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 11, 2020, 09:40
Default
  #8
New Member
 
John Applesmith
Join Date: Feb 2020
Posts: 13
Rep Power: 6
ns778 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Most functions in CFX can be done using CEL and do not need user fortran.

To get the maximum of this function at each timestep use the CEL expression:
maxVal(MyExpression)@Domain Name

Look in the CFX Reference manual for the other available CEL functions and expressions.
Hi, I tried your method and got the following error

"The function 'maxVal' referenced by parameter 'Expression Value' in object '/FLOW:Flow Analysis 1/OUTPUT CONTROL/MONITOR OBJECTS/MONITOR POINT:transPress' has an invalid argument, 'Absolute Pressure.Time Derivative'. The solver does not support the use of this operator for this variable when used as an argument for this function.

I get similar messages no matter where I try to create the function- Set-Up CEL, as Monitor Point or in Post. The formula I'm using- maxVal(Absolute Pressure.Time Derivative)@tubeFluid. Even when I define the pressure transient separately and pass it into maxVal. What does work is Absolute Pressure.Time Derivative on its own.
ns778 is offline   Reply With Quote

Old   May 11, 2020, 10:40
Default
  #9
Senior Member
 
Join Date: Jun 2009
Posts: 1,815
Rep Power: 32
Opaque will become famous soon enough
As a workaround, you can always copy a valid variable into an Additional Variable (which usually works everywhere else),

Create an additional variable: (unspecified) with units = [Pa s^-1]
Activate the additional variable within a domain
Select Algebraic Additional Variable
Set it equal to = Absolute Pressure.Time Derivative

Try using the Additional Variable in those places you need it,
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 14, 2020, 13:08
Default
  #10
New Member
 
John Applesmith
Join Date: Feb 2020
Posts: 13
Rep Power: 6
ns778 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
As a workaround, you can always copy a valid variable into an Additional Variable (which usually works everywhere else),

Create an additional variable: (unspecified) with units = [Pa s^-1]
Activate the additional variable within a domain
Select Algebraic Additional Variable
Set it equal to = Absolute Pressure.Time Derivative

Try using the Additional Variable in those places you need it,
Worked perfectly- thank you so much!
ns778 is offline   Reply With Quote

Reply

Tags
post, pressure transients, results

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
[Other] mesh airfoil NACA0012 anand_30 OpenFOAM Meshing & Mesh Conversion 13 March 7, 2022 17:22
static vs. total pressure auf dem feld FLUENT 17 February 26, 2016 13:04
[blockMesh] error message with modeling a cube with a hold at the center hsingtzu OpenFOAM Meshing & Mesh Conversion 2 March 14, 2012 09:56
seeking for help about a room with negative pressure mengyue1 FLUENT 0 November 26, 2009 06:40
negative pressure mAx FLUENT 0 January 25, 2006 14:31


All times are GMT -4. The time now is 06:57.