# dp vs. flow

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 August 23, 2007, 11:45 dp vs. flow #1 Wooster Guest   Posts: n/a I have a model that I've been having problems with. at low flows (1 gpm) it syncs up with lab results quite well on a square root DP vs. Flow chart. However, as the flow goes up, the curves diverge. For example at 5 gpm the data point is 20% off of the accepted value. I've run a mesh study and examined my y+ values and found little to no problems with it. I'm wondering if the problem is within my turbulence calculation and if so, there is a bewildering forest of check boxes, values, etc. that I would need to check. I'm using k-e, and SST but they give me pretty much similar issues. Before I wander around in the dark, is there some experience you guys have in this and perhaps I'm just missing some crucial check box? -W

 August 23, 2007, 16:01 Re: dp vs. flow #2 Stumpy Guest   Posts: n/a Do you have a boundary condition specified using units of [gpm]? If so this is imperial gallons, [gpmUS] is US gallons.

 August 23, 2007, 16:24 Re: dp vs. flow #3 Wooster Guest   Posts: n/a The inlet condition is mass flow in lb/sec. I just chart it in gal/min for the ease of the other colleagues. I use the conversion for US gallons (8.33). The outlet is avg pressure of 0 psi. -W

 August 23, 2007, 18:15 Re: dp vs. flow #4 Glenn Horrocks Guest   Posts: n/a Hi, Have you reproduced the experimental conditions accurately enough (probably not if your answers are diverging). Things to consider include velocity profile - is it fully developed or some other profile, initial turbulence - what is the inlet turbulence level, upstream pressure measurement - experimental pressure measurements are usually done effectively at a point, have you used the same point and considered whether it was measuring the static pressure only or whether a dynamic component would be included? Glenn Horrocks

 August 24, 2007, 11:10 Re: dp vs. flow #5 Wooster Guest   Posts: n/a My input to CFX is no velocity profile with a 5% intensity turbulence value. At the point where the model begins, this is a good approximation after having stretched the inlet to a L/D of 10 and checked the dp's between the two models. The experiment used a static dp sensor and the CFX model describes the entire setup 100% right down to the fittings, pressure sensing point, etc. You are the second person to say that the divergence is a physical model issue which prompts me to visit the machinist to make sure my drawings aren't outdated or he didn't put some twist in the thing he never put to paper. I doubt it though as I've seen the model taken apart (and cleaned). Thanks! -W

 August 28, 2007, 08:39 Re: dp vs. flow #6 Johnson Guest   Posts: n/a You don't say what fluid you are using in your experiment - is it water (i.e. incompressible)? If not, compressibility effects are sure to play a part at higher flow rates. Also, is the pipe rough or smooth? I might also question the assumed L/D ratio to generate a fully developed velocity profile. If the analysis is isothermal, you could try modeling a small length and applying a pressure drop/mass flow using a Domain Interface. Johnson

 August 28, 2007, 18:20 Re: dp vs. flow #7 Glenn Horrocks Guest   Posts: n/a Hi Wooster, What are you actually modelling? I assume it is some sort of valve or pipe fitting you want a pressure versus flow rate curve for. Glenn Horrocks

 August 29, 2007, 10:45 Re: dp vs. flow #8 Wooster Guest   Posts: n/a Glen, Well, its a lot more difficult than that. I'm modeling an ion beam target with cooling fluid flow in a fairly complex geometry of tight bends, very small tubes (0.055"), and an immersed jet where the fluid does a 180 back up around the nozzle to a swagelok tee fitting. The goal is to benchmark this fabricated piece such that we can derive loss coefficients, and heat transfer coefficients for a industry specific mathematical model. I've broken the paths down to elementary pieces (as much as possible) and checked them with pen/paper calculations where possible to comprise a good mesh study. I had to blend out the second order approximation ever so slightly to get the jet problem to converge. Right now, I'm chasing down meshing resolutions at the point where the fluid goes from a relatively large annulus to tiny tubes. The area where the water flows into much smaller tubes is the key suspect at the moment thus I need to make sure that the mesh (which has been tested successfully to work on individual pieces) works when the pieces are put together. I'll run a couple of simple mesh studies (later in the week) on the corner to determine if I need to blend the mesh sizes even further than what I have already done. Just FYI, The benchmark test piece was tested in clinical conditions using a calibrated DP and flow sensor. I've taken the original apart (I designed about half of it myself) to see if there was anything major that would cause the results to have a different trend, but unless there is something stuck in the 0.055" tubes that no one can see, my CAD model is about as close to reality as it's feasible to be. Thanks a bunch for the help! -W

 August 29, 2007, 10:51 Re: dp vs. flow #9 Wooster Guest   Posts: n/a Johnson, The fluid is water with smooth tubing (this is taken into account in the data). I'll take a look at your isothermal suggestion. Thanks! -W

 August 29, 2007, 18:53 Re: dp vs. flow #10 Glenn Horrocks Guest   Posts: n/a Hi, Just a thought - could the additional pressure at high flows be causing the geometry to distort? I have no idea if your pressures are high enough for this to happen but it is worth asking. Some other ideas: Maybe you get laminar/turbulent transition effects at higher flows? Does a separation bubble make a fundamental change in behaviour which is not being captured properly in the CFD? Maybe you enter a region of wake vortex shedding and that changes things. Glenn Horrocks

 August 30, 2007, 13:17 Re: dp vs. flow #11 Wooster Guest   Posts: n/a Glenn, The material is usually Tantalum (Ta on the charts) and is extremely hard to bend. As for turbulence, even low flows of 1 gpm require some k-e/SST/etc. The RE number is way too high for laminar type flows. As for the bubble.....now that is something I've thought of before but I can't think of anyway to test that assumption. My colleagues and I can't think of anything that would cause a bubble to get stuck in key places since the DP of the system is high enough to sweep just about anything through. This doesn't mean that it can't happen. My next set of steps will be to try and mimic a bubble in the flow. I think I can do this by effectively blocking a channel and see how my DP's respond. Other than that, I'm going to start examining various DP's through the system as solver iterates. If one is changing drastically, then that may signify some problems. Normally everything settles out within 20 or so iterations Thanks for the help! Mark

 August 30, 2007, 18:48 Re: dp vs. flow #12 Glenn Horrocks Guest   Posts: n/a Hi, I am not talking about a physical bubble (ie air bubble or whatever) - but if that is a possibility then maybe you should investigate it. What I was trying to say is that maybe as the flow rate increases maybe a new separation occurs, or maybe an existing separation grows and intersects with something else - maybe a cross hole or whatever. This might require some new physics to model and the turbulence model looses accuracy. Just a thought. Also consider swirl. Is there significant swirl which increases with flow rate? The 2-equation turbulence models do not model swirling flows very well and loose accuracy quickly. Glenn Horrocks

 August 31, 2007, 10:56 Re: dp vs. flow #13 Wooster Guest   Posts: n/a Glenn, I do see swirl in a couple of models I have and you're right, to model those requires some spade work with turbulence and equations (note my discussion on blend factors). I think I see what you're saying about a bubble. I'll give some other turb. models a try at the highest flow. I do have some pretty nasty turns and separation could be a likely cause. If nothing else, I'll get permission to post pics of the water volume for the entertainment (and possible amusement) of the audience. thanks again! -W

 August 31, 2007, 18:43 Re: dp vs. flow #14 Glenn Horrocks Guest   Posts: n/a Hi, Blend factor won't fix the swirl issue as it is inherent in 2-eqn turbulence models. The fix for swirl is to use higher order turbulence models such as RSM or move away from RANS turbulence models entirely and use LES/DES/SAS models. The SST model has a swirl correction thing which I think is a beta option. This may be of use if you wish to stay with a 2-eqn model (and I recommend you do if you can). Anybody know the CCL to turn it on? Glenn Horrocks

 September 1, 2007, 21:17 Re: dp vs. flow #15 Wooster Guest   Posts: n/a I believe you on staying with the 2 eqn models. I've tried some of the more "arcane" models packaged with CFX 11 and they had rather disastrous results (because I'm not familiar enough with them). I don't think the swirl is fixed with the blend. I re-read my post and could see how I might have confused you. The swirl isn't my primary concern and I've been able to see something of it with some SST models. The primary area I believe requires the blend is in the momentum as the water makes a tight 180. The swirl actually comes into play after this region. I might be wrong (I'm no expert) but something about that jet model does not like a 100% second order approximation. A study has shown it likes a blend of 0.89. Now this doesn't take into effect time scales and that is the work for this week. -W

 September 3, 2007, 09:14 Re: dp vs. flow #16 Juan CatelĂ©n Guest   Posts: n/a I think that in this kind of case you should use Omega Reynols Stress. I have got amazing results (comparing with experimental data and correlations for dp). The problem is that you need a very heavy mesh. Bye.

 September 4, 2007, 11:23 Re: dp vs. flow #17 Wooster Guest   Posts: n/a Heavy Meshes are my specialty. Usually mine are around 5 million nodes and counting. Horrific large files. -I'll give the model a shot. Thanks! -W

 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 CD adapco Group Marketing Siemens 3 June 21, 2011 08:33 saii CFX 2 September 18, 2009 08:07 James Main CFD Forum 6 May 15, 2009 12:14 curious ... Main CFD Forum 23 July 21, 2006 07:40 Franck Main CFD Forum 3 September 4, 2003 05:57

All times are GMT -4. The time now is 14:34.

 Contact Us - CFD Online - Privacy Statement - Top