
[Sponsors] 
January 12, 2007, 16:27 
converge problem

#1 
Guest
Posts: n/a

Sponsored Links
I'm a first time CFX user. I'm running a valve simulation. Now, when the mass flow rate is high, it converges very well. When the mass flow rate is reduced, it always diverges. The valve inlet dia. is 6 mm, outlet dia. is 4mm. Some restrictions in between. And, the inlet BC: subsonicâ€"total pressureâ€"normal to boundary conditionâ€"turbulent option is medium (5%) Outlet BC: subsonicâ€"mass flow rate Wall BC: No slipâ€"smooth Global initial guess are all "automatic" except I input the velocity component values. HT model is Isothermal and Turbulence Model is KE. The fluid is liquid. For 0.1 kg/s or higher, it converges very well. For 0.05 kg/s mass flow rate or lower, it diverges. I changed the turbulence to low (1%), it doesn't help. I used the 0.1 kg/s result as the initial guess for the 0.05 kg/s case, it cannot converge either. Are there any way to try? Thanks in advance. Snowshovel 

Sponsored Links 
January 12, 2007, 16:33 
Re: converge problem

#2 
Guest
Posts: n/a

BTW, I'm still trying to use Physical Timescale and make the value less than the automatic value to try my luck.


January 13, 2007, 01:17 
Re: converge problem

#3 
Guest
Posts: n/a

Did you try refining your mesh?


January 14, 2007, 08:51 
Re: converge problem

#4 
Guest
Posts: n/a

use LES


January 14, 2007, 12:12 
Re: converge problem

#5 
Guest
Posts: n/a

Hi snowshovel,
Did you already refined the mesh near the walls? I don´t know what kind of fluid you use but perhaps you should use a kw Model to simulate low massflowrates. Have a look at the CFX Help. Thomas 

January 15, 2007, 04:06 
Re: converge problem

#6 
Guest
Posts: n/a

Dear Mr. Snowshovel,
How did you decide the Total pressure at inlet. Best Regards Eric my email: qiuyifa@hotmail.com 

January 15, 2007, 12:36 
Re: converge problem

#7 
Guest
Posts: n/a

Thanks all for the kind reply.
Yes, I'm using a very fine mesh. The Y+ value is less than 10. I assume it's fine enough for a kE model. As far as the total pressure BC Eric indicated, it's a test data far upstream where the fluid velocity is very low. So I assumed it as a total pressure at the inlet. My interest is the relationship between the pressure drop across the valve and the valve mass flow rate. So, I can figure out an equation for the effective area calculation that can be used for 1D programming. Am I doing something wrong with the BC definition? Would a static pressure help the converge? I'm not an expert on CFD, especially on CFX. It seems that the CFX auto timescale is calculated by factor (0.3) times the L/V (I'm not sure about this, for my cases, the auto timescale is close to this hand cal.). This auto timescale is fine for the high mass flow rate in my case, however, it's too big for the low mass flow rate case. I just made one case converge with a much smaller physical timescale. Moreover, it seems I need to use the small physical timescale from the very beginning, not in the middle. I'm still trying some smaller mass flow rate cases. Except this problem, anybody knows how to measure the dimensions in CFX, for example, the diameter? I did choose the right dimension when I import the mesh from ICEM CFD. And, from the bottom of the CFXPre window, the dimensions look right. However, I still wanna check the dimensions inside. I cannot read the CFX help because of JAVA, maybe, problem (from the answer for the "HELP" problem in this forum). Hopefully, I won't have so many problems after I can read it. Thanks all again. 

January 15, 2007, 14:39 
Re: converge problem

#8 
Guest
Posts: n/a

Hi Snowshovel,
You can access PDF help files in the CFX installation under .../help/pdf. To check your model dimensions, plot X, Y, or Z on one of your surfaces in Post. It seems very unusual that your model diverges at the low mass flow rate. It is not often that CFX diverges at all when solving simple hydrodynamics (complex physics, perhaps). In nearly every case that it does, the problem is an unphysical boundary condition, wrong mesh scale or very poor mesh quality. I'm not suggesting that you have done something wrong, but this is the common behavior. I suggest writing backup files just before the solver blows and looking at where things are going wrong. The mass or energy equations are usually first to go, so look for regions of very high pressure or temperature. If these occur where you would not expect it, you at least know where it is going wrong and can look for bad elements, if any, or better understand the process that is leading to the divergence. Your assumptions on the total pressure inlet seem reasonable. If you have measured static pressure in a plenum or very low velocity region upstream, it is appropriate to use total pressure at your inlet. I would say that there are very few cases where a static pressure inlet is of any use. A couple other thing worth trying are: 1. Run the solver in double precision. No guarantees here, but it is sometimes the "majic" solution, particularly if poor grid is the issue. 2. Reduce the inlet turbulence level in the low mass flow case. Make sure that these numbers are sensible. Also verify that the flow is indeed turbulent for these cases. Calculate the Eddy Viscosity Ratio in Post (EVR = Eddy Viscosity/Dynamic Viscosity), EVR should be >>100 throughout most of your domain. 3. Set the initial guess to "Automatic" for everything and let the solver initialize the flow. I've seen a lot of good intentions cause problmes that go away when the solver is left to do it's thing. 4. You can try specifying a larger or smaller timestep, but don't go too far at either end (a very small timestep can also cause problems). Timescale should be within two orders of magnitude of the advection time. The solver estimates this by dividing the cube root of the volume by the average velocity scale (well, there is a little more to it than that...) and using 1/5 of the calculated value. If any of this helps or you find a solution, let us know what worked. Don't be afraid to contact technical support either, even if you are an academic user. Academic support is low priority, but someone may help you if they have the time. Regards, Robin 

January 15, 2007, 18:07 
Re: converge problem

#9 
Guest
Posts: n/a

Hi, Robin,
Thank you very much for your suggestion. I can access PDF HELP files and check the geometry now. My model is that the fluid flows into the domain axially, then hits a plate. So the flow direction will become normal to axis along the plate surface (the plate is normal to the valve axis). After passing some ports on the plate, the fluid will merge somewhere after the plate and flow out of the valve axially again. Just checked the EVR value you suggested. The value in most of the domain is below 100 (around 49.XX). This case stopped the running after the RMS values for u,v,w,pmass are lower than 1E04 that I defined (I used a small physical timescale). However, the RMS values for KTurbKE and EDiss.K are still higher than 1E04. Should I switch from the ke model to SST? 

January 15, 2007, 18:24 
Re: converge problem

#10 
Guest
Posts: n/a

hit the "post message" accidentally.
For flows in a complex geometry component, what criteria we should use to decide to use a turbulent model (Re range)? For low Re flow, kw model should be better than ke. My question is how accurate in CFX the kw models (baseline kw and SST kw) is (robust and easy to convege)? Thanks in advance. 

January 16, 2007, 12:58 
Re: converge problem

#11 
Guest
Posts: n/a

Hi Snowshovel,
The turbulence equations can often have very high residuals and are not included in the convergence criteria, so there is no need to worry about their convergence level. Komega models are not necessarily better than ke models at low Reynolds numbers. They are sometime referred to as lowRe models, but this is referring to the boundary layer treatment, not the flow Reynolds number. A low Eddy Viscosity Ratio may indicate that your flow is not fully turbulent and the turbulence treatment may not be appropriate. You could try running a laminar solution, but this may not be entirely appropriate either if the flow is transitional. CFX has a turbulent transition model, but I would review the literature first to see if this is appropriate for you case. In the end, you may just have to leave out the low flow cases. Regards, Robin 

January 16, 2007, 15:23 
Re: converge problem

#12 
Guest
Posts: n/a

I've a question for Robin..how low has to be the Eddy Visosity ratio of the flow to be considered as laminar?
Thanks, Andres 

January 17, 2007, 14:11 
Re: converge problem

#13 
Guest
Posts: n/a

Hi, Robin,
Thank you very much! I did learn a lot from your suggestions. Please let me know what's your comment on the transition model in CFX. Best regards, Snowshovel 

January 18, 2007, 22:05 
Re: converge problem

#14 
Guest
Posts: n/a

Hi Andres,
It's not that the flow is laminar or not. The problem is that the assumptions (and more importantly the simplifications) of the turbulence models are no longer applicable in these situations. How strongly this affects the accuracy will depend on your particular model. I'm not an expert on turbulence, so I hesitate to comment further. Regards, Robin 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Handling cyclic BC from gambit to openfoam for a cascade airfoil problem  OF 1.6  maverick  OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...  2  June 18, 2011 04:36 
Velocity profiles problem behind the elbow (3D problem)  kabat73  FLUENT  8  May 9, 2010 04:26 
Adiabatic and Rotating wall (Convection problem)  ParodDav  CFX  5  April 29, 2007 19:13 
Converge problem of 3D free jet flow  Jen  FLUENT  11  January 24, 2005 01:21 
problem with using colocated code  Jack  Main CFD Forum  0  December 15, 2002 01:15 
Sponsored Links 