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

general momentum source/hydraulic pressure jump/positive displacement machine

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 28, 2009, 21:30
Default general momentum source/hydraulic pressure jump/positive displacement machine
  #1
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
I need some help in setting up a momentum source. I want to model an internal flow system that contains throttles and a positive
displacement machine. I want to see the effects of the positive displacement machine in the system, however I'm not interested
on modeling the actual machine in 3D but a reduced mathematical model. I have the machine performance curves (speed, pressure
ratio, volume flowrate, icentropic efficiency etc. Therefore I have created a general momentum source with a simple array that
relates dp with flowrate for testing. As for BC inlet is relative pressure 0 [Pa] and outlet's velocity 5 [m/s] (will be massflow
later to match the real problem setup but should be ok for now)

FUNCTION: DpQ
Argument Units = [Pa]
Option = Interpolation
Profile Function = Off
Result Units = [m^3/s]
INTERPOLATION DATA:
Data Pairs = 0,0.025,500,0.05,1000,0.075
Extend Max = On
Extend Min = On
Option = One Dimensional
END
END

#density = 1.284 [kg/m^3]
#duct area = 0.05 [m^2]

Pin = massFlowAve(p)@F91.89 2
Pout = massFlowAve(p)@F96.89 2
deltaP = abs(Pout-Pin)
velocity = volflow/area@F96.89 2
volflow = DpQ(VardeltaP)
#the variable VardeltaP is the algebraic expression deltaP

scoef5 = -10e5 [kg m^-3 s^-1]
svalue5x = scoef5 * (Velocity u - 0[m/s])
svalue5y = scoef5 * (Velocity v - 1[m/s])
svalue5z = scoef5 * (Velocity w - 0[m/s])

When I use the above basic source definition I can get the thing to converge with the specified velocity in the defined subdomain
but when I use the equations below there are many issues:

scoef5b = Density * volflow / volume()@B89 2
svalue5bx = scoef5b * (Velocity u - 0[m/s])
svalue5by = scoef5b * (Velocity v - velocity)
svalue5bz = scoef5b * (Velocity w - 0[m/s])

a) for example cfx-post wont let me evaluate the velocity and volflow scalars so I dont know if my coefficient is calculated
correctly.
b) the problem converges but velocity has the value from the outlet boundary and pressure's are..... well wrong
IN = -1.655e+01 [Pa]
OUT= -1.547e+02 [Pa]
dp across subdomain = -1.381e+02 [Pa]
c) am I doing something wrong with my problem approach? I would appreciate any comments especially if the source coefficient is
properly defined and if the expression volflow = DpQ(VardeltaP) is correct.

many thanks
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   June 28, 2009, 22:55
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

I would not use "velocity" as a CEL variable. It might get corrupted with the internal velocity variable. Use a different variable name.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   June 29, 2009, 05:09
Default
  #3
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Hi,

I would not use "velocity" as a CEL variable. It might get corrupted with the internal velocity variable. Use a different variable name.

Glenn Horrocks
didnt make any difference mate - the variable is case sensitive anyway so its should be ok - however I changed it anyway to test it.

However in cfx-post I do get the follwing error "The following unrecognised name was referenced: DpQ." thats the only bit that I'm unsure, the definition of the volflow expression as the function calculates at the pressure diferential at the inlet and outlet of the subdomain and then it should look up the pressure diferential from the array and output the volume flowrate.

I attach the full ccl if anyone has the time to check and comment
Attached Files
File Type: txt CFX12_source_velocityb_vel.ccl.txt (5.9 KB, 37 views)
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   June 29, 2009, 18:30
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Some issues I can see:

You refer to "Density" in scoef5b. This is not defined.
You define velocityx = volflow/area@F96.89 2. It should be area()@F96.89 2
You have no materials defined. Did you snip that out of the CCL? You need to have some materials defined.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   June 29, 2009, 18:35
Default
  #5
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
materials is the stanadrd air @ 25 [C] mate (was a bit lazy ) I just copy paste the expression ccl code and forgot materials but use the standard ones for the example

Density is the variable name for density of the fluid m8 EDIT: yes stupid of me density but where its located thanks I got it now

just checking the area()@
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   June 29, 2009, 18:57
Default
  #6
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
fixed the mistakes and cfx finds a solution but I still get still wrong results which means there is still something else wrong as I still get the "The following unrecognised name was referenced: DpQ." in cfx post

The 1D array is there but maybe there is another way to write the volflow = DpQ(VardeltaP) expression
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials

Last edited by ckleanth; June 30, 2009 at 04:36.
ckleanth is offline   Reply With Quote

Old   June 30, 2009, 17:49
Default
  #7
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
still bugging me this flippin expression
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   June 30, 2009, 18:57
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Sorry, did not read your initial post fully - I don't think CEL interpolation expressions are sent to CFD-Post. The best way to check where on your curve your function is lying is to set up monitor points for the input and output of the expression then you can export them from Solver Manager and check them externally.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   June 30, 2009, 19:03
Default
  #9
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
thanks mate will try this tomo..

if I remember correcly fluent had this setup as ready made BC ...
cant be that hard of a thing to do really... cant see any other way to model loads of fans/pumps inside a system using the machine characteristics...
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   August 24, 2012, 16:29
Default
  #10
New Member
 
Philippe Vidori
Join Date: Apr 2011
Posts: 8
Rep Power: 6
philflow is on a distinguished road
Hello Sir,

I'm going through the same problem at the moment. Just curious to see if your model worked in the end.

Best regards,

Phil

P.S: CFX is a pain with fans !!
philflow is offline   Reply With Quote

Old   August 25, 2012, 06:23
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Several post on this forum talk about this technique to model fans. It is quite commonly done and works fine when set up correctly.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Porous domain vs Subdomain General Momentum Source alvio CFX 1 November 18, 2008 16:44
total pressure drop and momentum source setting Li CFX 2 July 28, 2008 02:33
How to apply negtive pressure to outlet bioman66 CFX 5 June 3, 2006 01:40
general momentum source in cylindrical direction Atit CFX 1 May 31, 2006 09:05


All times are GMT -4. The time now is 05:58.