# Boundary conditions race car charge air cooler

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

 March 5, 2013, 04:16 Boundary conditions race car charge air cooler #1 New Member   Join Date: Mar 2013 Posts: 4 Rep Power: 6 Greatings forum, we are a group of students that work on a bachelor thesis in Sweden. We are doing simulations in CFX on different parts of a charge air cooler in a race car. We have read threads on this forum several times to get some help but this time we need to make a post about it. We are currently simulating the housings that distributes the air from a tube to a rectangular shape (similar to an air intake manifold). We have an known inlet pressure in the tube but we cant seem to get the outlet boundary condition right... We want to look at the pressure distribution at the outlet. The outlet consists of several small channels. I Hope that anyone understands the problem since I cant write to much details about it.

March 5, 2013, 07:14
#2
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Quote:
 We have an known inlet pressure in the tube but we cant seem to get the outlet boundary condition right...
What do you mean by this exactly? Have you tried with different options and it diverges? Is the flow subsonic, supersonic, compressible, incompressible? An image of your flow domain may shed some light on the problem definition.

Typically, if the inlet static pressure conditions are specified, and if outlet velocity is known, you can specify it as normal speed at all bunch of outlets. This way the outlet pressure can be obtained. I also find the somewhere mentioned that it is robust way to specify total pressure at inlet and velocity/mass flow at outlet to get static pressure at outlet. But not sure if it is good practice for subsonic incompressible flow.

OJ

March 5, 2013, 08:41
re
#3
New Member

Join Date: Mar 2013
Posts: 4
Rep Power: 6
We have a inlet pressure of 2.3 bar and a mass flow of 0.24 kg/s. the flow is subsonic and we have used a inlet boundary as "inlet-static pressure" and for the outlet boundary we have tried "opening-Pres. and Dirn" and "Outlet-Average Static Pressure" (using pressure averaging etc that we read about in the guide" and several other B.C's in opening and outlet. But the results dont seem to be any good since all our attempts give us a uniform pressure over the outlets but it should be a difference since thats whole point of our simulations.

I have attached some images from CFX-post. as You can se the pressure is almost uniform and we are expecting a non uniform pressure distribution. This is to evaluate which housing gives the most even pressure across the outlets.

Attached Images
 Figure001.png (25.2 KB, 18 views) Figure002.png (46.6 KB, 14 views) Figure003.png (74.8 KB, 13 views) Figure004.jpg (27.8 KB, 11 views)

 March 5, 2013, 20:03 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,097 Rep Power: 109 Make sure you use a reference pressure so the pressure boundary condition can be 0Pa.

 March 6, 2013, 03:20 #5 New Member   Join Date: Mar 2013 Posts: 4 Rep Power: 6 Thx for your replays, ghorrocks do you mean to put the reference pressure in the fluid domain to 2.3 bar (that is our inlet pressure) and then use 0 pa in outlet and 2.3 bar in the inlet? or do we put 1 atm ref pressure in the domain and 2.3 bar in the inlet and 0 pa in the outlet ?

 March 6, 2013, 18:39 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,097 Rep Power: 109 I do not understand the two options you explain. Put the reference pressure at the outlet pressure, and the inlet at its pressure relative to that.

March 7, 2013, 05:39
#7
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Quote:
 as You can see the pressure is almost uniform and we are expecting a non uniform pressure distribution. This is to evaluate which housing gives the most even pressure across the outlets.
If you carefully observe the pressure contours at the outlet channels, you will realise that the scale used ranges from -3e9 to 1.8e9 Pa. If you take this big scale, obviously the pressure will appear uniform!

If you want to see the better resolution of pressure distribution, you should use a smaller range.

OJ

 March 7, 2013, 05:47 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,097 Rep Power: 109 Good point OJ. But probably more important is that this range of pressure is unlikely to be physically possible - does your header handle GPa of pressure? I don't think so.... So you have a fundamental error in your simulation to generate such large pressures. Your flow is probably too high, or you are using the wrong material, or you need to use a compressible gas or some other fluid property which will bring the simulation back to reality.

March 8, 2013, 05:08
#9
New Member

Join Date: Mar 2013
Posts: 4
Rep Power: 6
Once again thank you guys for the help!

Yesterday we got some results that may be "good"

We are using a single domain and have an inlet and an outlet. The Domain is air, ideal gas at 175 C and the reference pressure is 2.3 bar in the domain.

The inlet is defined as inlet with static pressure of 2.3 bar.
The outlet is defined as outlet with mass flow rate of 0.24 kg/s (no definition for the pressure here)

We also looked more on the scales of plots and found that tips very helpful.
Im posting some results for you to look at if you want to. We are meeting with our supervisor later today to discuss these to se if they are liable.

If you are wondering why the outlets are elongated, we read somewhere that you want to elongate the exits to get a good result so we made the exits 100m but in the plane plot we show the pressure at 0mm (close to the housing).
Attached Images
 Figure001.jpg (38.4 KB, 10 views) Figure002.jpg (33.4 KB, 8 views) Figure003.jpg (36.4 KB, 8 views) Figure004.jpg (65.3 KB, 8 views) Figure005.jpg (50.2 KB, 7 views)

 March 8, 2013, 07:54 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,097 Rep Power: 109 Some comments: * Make the inlet 0Pa and use a reference pressure of 3.3bar (assumign your 2.3bar is gauge). * Something funny is going on with the first outlet. It does not look right that it has a much different flow the every other one. * That dirty big circulation is bad. Either your simulation is not converged and it is nto real; or your simulation is converged the circulation is real and your design is poor. Circulations = loss and big circulations = big loss. * Have a think about what you are trying to do. You want to slow the flow down, and then squirt it evenly down the multiple pipes. To slow a flow down you need a diffusor - but you have a convergent duct. I suggest you redesign the header to include a diffusor to slow the flow down with minimum losses.

 March 8, 2013, 10:32 #11 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 13 I understand that the rationale for the exercise is to have a uniform pressure distribution over outlet. Essentially, this means there has to be close-to-uniform distribution of flow in the outlet channels. Now, if you see the shape of the your casing, the outlet manifold tapers at the region before outlet channel. This results in increased back pressure at the tapered area. Essentially, the pressures at the beginning of all your outlet channels will be non-uniform, making the final outlet pressure non-uniform. In addition to Glenn's suggestion, would it also make sense, to do a 2D analysis of this section, to judge how the shape should be, before escalating it to 3D? The best design (and simulation) practices are all about tackling challenges one by one, so you are prepared to understand and address the questions at most complex phase of your journey OJ

 Tags boundary, cfx, conditions, outlet, problem

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post HMR CFX 5 October 10, 2016 05:57 Thomas P. Abraham Main CFD Forum 20 July 7, 2013 05:05 mehrdadeng CFX 10 February 25, 2011 06:25 Paolo Lampitella FLUENT 0 June 12, 2008 06:25 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15

All times are GMT -4. The time now is 10:52.