
[Sponsors] 
What to Do When There is a Large Scale Difference in Geometry? (too large/small dom.) 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 14, 2019, 08:05 
What to Do When There is a Large Scale Difference in Geometry? (too large/small dom.)

#1 
New Member
yanki
Join Date: Sep 2016
Posts: 7
Rep Power: 5 
I want to simulate the leakage inside a pipe.
The problem is, pipe has a 20 mm diameter whereas crack has a 0.05 micrometer diameter and the crack length (pipe thickness) is 4.1 mm. So after geometry creation I cant even see the leakage domain because it is almost nonexistent compared to the pipe domain. I'm thinking about partially modeling the area of interest but how? Anyone has any idea? 

June 14, 2019, 09:20 

#2 
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 55
Rep Power: 2 
I have never modelled such thing (I think some kind of Boolean needed to subtract crack from rest of geometry) but if you create different blocks (for mesh)you can have different domains to work with. You will not lose even tiny things.
Even creating 'Part name' at time when you create crack can help but it will be in same domain. 

June 15, 2019, 15:25 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,779
Rep Power: 121 
As you suggest it is difficult to model things with large differences in length scales.
Can you explain what you are modelling? Why do you need to model the pipe and the crack at the same time? Why can't you just model the crack by itself? And the pipe by itself? Can't you simulate the crack with a model of just the crack using a pressure from the pipe model, and the pipe is modelled using a mass sink at the crack location?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

June 17, 2019, 09:17 

#4 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 872
Rep Power: 17 
Glenn is correct (as always).
I would figure out what the flow parameters of the crack would be first. Develop a curve for DP vs flow. This may end up looking like an orifice calculation, with you discharge coefficient and area. Then in you pipe model, use a point source with your flow curve, which would act as a mass source or sink if you make it negative. 

June 21, 2019, 12:50 

#5  
New Member
yanki
Join Date: Sep 2016
Posts: 7
Rep Power: 5 
Quote:
Quote:
Quote:
Guys, I tried to draw a sketch for the explanation. Yellow circle is the area of interest. While from this sketch it looks simple but diameter of the crack hole is 0.05 micrometer and length is 4100 micrometer, almost half million times of it. Basically we have a tube and inside this tube there is a flow with 500 bar. Pipe outlet have atmospheric pressure. I tried to solve it by taking a portion of the domain. However there are some problems. 1) What pressure value should I enter at the outlet of this cube domain? Atmospheric pressure, same as full model? Because in reality inlet and outlet of this small area of interest is very close to each other. 2) When I increase the diameter of this crack, pressure drop increases, normally opposite of this should occur? 3) This is interesting, when I plot the velocity contour, I see very big velocity values inside this domain. Normally, this domain is already very close to the wall, so CFX basically consider this domain as its own and calculates a new boundary layer and a new velocity profile. I would expect near zero velocities inside this domain. 3) Most of the fuel evaporates just in front of the inlet of the crack and cannot reach to the surface (I see some small mass flow rate values at the outlet like 9x10e23 kg/s). While it is possible, then how should I calculate the pressure drop vs Length of the crack. And most importantly will there be a leakage? Because when I tried to just model the crack geometry alone, then the domain becomes full of fuel, so what comes in through the inlet also goes out from the outlet? 4) Leakage test is done under hydrostatic pressure, so basically they inject the fuel (or N2) with high pressure and close everywhere. So maybe I should use mass flow inlet for those symmetry walls as well? Because in a hydrostatic test condition, there will be no flow, just a static pressure everywhere? Last edited by yanqoue; June 21, 2019 at 19:10. 

June 23, 2019, 21:50 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,779
Rep Power: 121 
This crack is so small that it is likely to be smaller than the boundary layer, and maybe the size of the laminar sublayer. This means that the fluid at the entrance to the crack is essentially stationary. If this is the case then the crack can be modelled with stationary flow at the pressure end and just a pressure inlet.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

June 24, 2019, 00:12 

#7  
New Member
yanki
Join Date: Sep 2016
Posts: 7
Rep Power: 5 
Quote:
Didn't understand the last sentence. You mean I should just model the crack geometry with a cylinder? Then I would definitely see mass flow rate at the outlet because o conservation o mass. 

June 24, 2019, 04:37 

#9  
New Member
yanki
Join Date: Sep 2016
Posts: 7
Rep Power: 5 
Quote:
Thank you. One more question. As I increase the diameter, since the pressure is same in all cases (500 bar); 1) Velocity increases with the square of diameter increase. 2) Mass flow rate increases with the 4th power o diameter. Normally I would expect higher velocities on a pipe with smaller diameter. And non I'm trying to calculate the pressure drop and compare them, normally in a pipe with smaller diameter, pressure drop should be higher, but I get th opposite, these results don't make any sense to me. Am I missing something? 

June 24, 2019, 07:28 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,779
Rep Power: 121 
Increase which diameter? Which velocity increases? Which mass flow rate increases? Please make sure you explain what you are talking about.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

June 24, 2019, 07:30 

#11 
New Member
yanki
Join Date: Sep 2016
Posts: 7
Rep Power: 5 

June 24, 2019, 13:47 

#12 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 872
Rep Power: 17 
Mass flow should vary with diameter to the 4th power. This is simple laminar flow theory through a pipe. Velocity should do the same (square of the diameter increase)
Just do a simple laminar flow calculation with friction factor = 64/Re, and you will see this is expected. 

June 24, 2019, 14:23 

#13  
New Member
yanki
Join Date: Sep 2016
Posts: 7
Rep Power: 5 
Quote:
Then, I'm getting the same pressure drop because pressures are input parameters. Since we have 500 bar inlet pressure and 0 bar outlet pressure, pressure difference will be same in all cases (500 bar difference), even the pressure drop vs length curves will be same. So, we are about to solve this, last steps How should I proceed with this? If I simulate this with the way I showed in the sketch, I get cavitation (evaporation) in front of the crack, and no fuel reaches to the surface. Correct or not I can still get an answer for "amount of leakage?" question, which is "zero". But I know that this product will be tested under hydrostatic pressure, in that case we have no movement inside the domain just 500 bar acting all over the place and in this situation the flow inside the domain will be different. This time there won't be a 90 degree flow working against leakage. In fact all of the liquid will try to move inside the crack. However If I try to model this with just crack geometry (cylinder), basically mass flow rate at the outlet will be equal to mass flow rate at the inlet, so I will %100 have leakage no mather what. is "What is the pressure difference inside the crack for various diameters in this system" question is a reasonable question? My manager asked me to find the leakage and the pressure drop, and don't know what to do now. Sometimes the simplest problem is the harderst one. 

June 24, 2019, 19:20 

#14 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,779
Rep Power: 121 
If the fluid is fuel (Diesel?) then you would expect this crack would cavitate. This means the fluid in the crack is either a gas, or a gas/liquid mixture. Either way it makes the analysis much more complex. This is not a trivial simulation, it will require careful thought.
There have been lots of modelling and experiments done on direct injection diesel injectors which would be relevant to this work. I recommend you do a literature study to find out how they handle the cavitation of the liquid.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
UDF value to large for defined data type  Anna73  Fluent UDF and Scheme Programming  9  September 30, 2018 22:18 
What method use to modelate a sideentry impeller in a large scale mixing tank?  fcabrales  Main CFD Forum  0  January 29, 2010 14:24 
large scale mesh motion  sb  FLUENT  1  April 27, 2007 22:23 
Large Scale Model:Small scale computer  gull  Main CFD Forum  0  March 5, 2007 06:37 
vitual _ real  deneb  FLUENT  3  January 22, 2007 04:31 