
[Sponsors] 
Closed volume pressure rise with temperature rise 

LinkBack  Thread Tools  Search this Thread  Display Modes 
January 11, 2016, 01:04 
Closed volume pressure rise with temperature rise

#1 
New Member
vinayak
Join Date: Oct 2013
Posts: 16
Rep Power: 8 
Hi,
I am trying to do isochoric compression CFD simulation in Fluent, i.e. a closed domain initialized with air, density as ideal gas law, zero static pressure, & 300 K temperature. I have defined constant energy source so as to increase air temperature, Now I want to observe rise in static pressure with temperature change. But while simulating I observe change in density & obviously in mass in closed domain instead of pressure rise. How can mass of air changes for a closed domain without any outlet? Please help me to sort out this issue. Thanks 

January 11, 2016, 14:50 

#2 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,828
Rep Power: 46 
Did you observe any pressure rise?
Is the density/mass rise significant? It may be an inconsistency (between your EOS, boundary conditions, and initial conditions) leading to a small rise in density. Try to run your simulation with the initial pressure & temperature and no energy source. And watch it develop. Use this to establish the true "initial conditions" that is consistent with all your modelling parameters. Then turn on the energy source. Do you have a localized heat source or is it volumetric? Density can change locally. 

January 13, 2016, 02:34 

#3 
New Member
vinayak
Join Date: Oct 2013
Posts: 16
Rep Power: 8 
Dear LuckyTran,
There is no any pressure rise. And Density (mass) of air goes on decreasing with increasing temperature due to heat source. I think for closed system mass, Volume & hence Density should remain constant. And as per ideal gas law (P=roh*R*T) , only Pressure should increase with temperature. But it is not observed in my case. 

January 13, 2016, 03:07 

#4 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,828
Rep Power: 46 
Probably an issue with your setup. What did you specify for boundary conditions? Are they adiabatic walls? What viscous model are you using? laminar?
Any fun findings with the no heat source simulation? 

January 13, 2016, 05:10 

#5 
New Member
vinayak
Join Date: Oct 2013
Posts: 16
Rep Power: 8 
Thanks LuckyTran For your quick reply.
I have modeled 0.1 m*0.1 m 2D closed air tank & 0.1 m depth value. All walls are adiabatic, air with ideal gas density, laminar model & 100 watt constant heat source. Operating pressure 101325 Pa. Case initialized with 0 Pa static guage pressure & 300 K temperature. Simple & 2 nd order schemes used. Firstly I run case in steady state , I get pressure as it is i.e. 0 Pa static guage, Temperature crosses its limit i.e up to 5000 K. & density decreased. When I switched same case for transient calculation, I got very realistic results. Density does remains constant, pressure & temperature goes on increasing with time. Results are exactly matched with hand calculation. I am surprised with steady simulation. I also gave convection BC in all walls Also stop heat source & give Temperature BC to one of the wall. But only Energy eq. is solved. And pressure remains stagnant while density drops. What should happen with steady CASE? 

January 13, 2016, 15:54 

#6 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,828
Rep Power: 46 
It sounds like you have solved your issue.
The pressure based solvers are generally segregated solvers (SIMPLE/PISO/etc). If you solve only the energy equation, the momentum equation is skipped. Because of the pressurevelocity coupling, the pressure is updated during the momentum equation (i.e. the flow equations). If you do not enable the flow equations, pressure will be fixed but temperature, density, and other material properties can still be updated. Hence with pressure fixed and increasing temperature, your density decreased because of the ideal gas law. If you had tried this problem using the COUPLED algorithm or density based solver you probably would have run into errors. You can freeze the velocity (via freezing variables method) if that is what you want to do but you need to enable the flow equations to get a new pressure. Last edited by LuckyTran; January 14, 2016 at 23:40. 

January 14, 2016, 23:31 

#7 
New Member
vinayak
Join Date: Oct 2013
Posts: 16
Rep Power: 8 
Thank you very much LuckyTran.


March 11, 2020, 02:50 

#8 
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 3 
@vinayak4399
After simulation, how to measure tank pressure?? Is it areaAvg(pressure)@tank_wall or areaAvg(pressure)@fluid ? 

March 11, 2020, 03:19 
Flow or NoFlow

#9 
Senior Member

If there is flow in the system, then it matters, otherwise, it does not matter.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 11, 2020, 07:46 

#10 
New Member
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 3 
So it there is a tank having inlet and outlet...then tank pressure = areaAvg(Pressure)@tank_wall..not areaAvg(pressure)@fluid..Right??


March 11, 2020, 08:29 
Objective

#11 
Senior Member

Then it depends on the objective. Pressure values will be varying across whole domain. Value at the boundaries is based on the solved flow field on the cells. The objective of doing the simulation will drive what information you need to get from the results. If you looking for whether the vessel or room can contain the pressure, then the pressure on the walls is important. If the pressure in the room is responsible for some other phenomenon, such as, particle dispersion, then pressure in the cell zone is more important.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how to set periodic boundary conditions  Ganesh  FLUENT  14  November 26, 2018 11:26 
Simulation of a single bubble with a VOFmethod  Suzzn  CFX  21  January 29, 2018 00:58 
Wrong flow in ratating domain problem  Sanyo  CFX  17  August 15, 2015 06:20 
Gas/liquid volume fraction function of pressure  bogild  ANSYS  0  September 25, 2014 09:11 
Hydrostatic pressure in 2phase flow modeling (long)  DS & HB  Main CFD Forum  0  January 8, 2000 15:00 