# converge problem

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

 January 12, 2007, 16:27 converge problem #1 snowshovel Guest   Posts: n/a Folks, 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 K-E. 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

 January 12, 2007, 16:33 Re: converge problem #2 snowshovel 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 Johnny Guest   Posts: n/a Did you try refining your mesh?

 January 14, 2007, 08:51 Re: converge problem #4 jehova Guest   Posts: n/a use LES

 January 14, 2007, 12:12 Re: converge problem #5 Thomas 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 k-w Model to simulate low massflowrates. Have a look at the CFX Help. Thomas

 January 15, 2007, 04:06 Re: converge problem #6 Eric Guest   Posts: n/a Dear Mr. Snowshovel, How did you decide the Total pressure at inlet. Best Regards Eric my e-mail: qiuyifa@hotmail.com

 January 15, 2007, 12:36 Re: converge problem #7 snowshovel 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 k-E 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 1-D 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 CFX-Pre 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, 18:07 Re: converge problem #9 snowshovel 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,p-mass are lower than 1E-04 that I defined (I used a small physical timescale). However, the RMS values for K-TurbKE and E-Diss.K are still higher than 1E-04. Should I switch from the k-e model to SST?

 January 15, 2007, 18:24 Re: converge problem #10 snowshovel 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, k-w model should be better than k-e. My question is how accurate in CFX the k-w models (baseline k-w and SST k-w) is (robust and easy to convege)? Thanks in advance.

 January 16, 2007, 12:58 Re: converge problem #11 Robin 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. K-omega models are not necessarily better than k-e models at low Reynolds numbers. They are sometime referred to as low-Re 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 Andres Bernal Ortiz 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 Snowshovel 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 Robin 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 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 maverick OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 June 18, 2011 04:36 kabat73 FLUENT 8 May 9, 2010 04:26 ParodDav CFX 5 April 29, 2007 19:13 Jen FLUENT 11 January 24, 2005 01:21 Jack Main CFD Forum 0 December 15, 2002 01:15

All times are GMT -4. The time now is 16:35.