
[Sponsors] 
April 8, 2011, 04:58 
Problems with increasing velocity with the time

#1 
Senior Member
Join Date: Mar 2011
Posts: 155
Rep Power: 7 
Hi,
I think I have two problems with divergence. One of them is that the solver crashed after a few time steps, but I don't want to discuss this one here. :) The other problem ist, that the solver solves the case, but the results are not very good. I'm solving with chtMultiRegionSimpleFoam an switched turbulence on. Now I want to see how velocity is solved. By setting the endTime to 100 there is a maximum velocity of about 30m/s. By setting the endTime to 500 there is a maximum velocity of about 200m/s. I have two inlets and two outlets. Inlet is set up with fixed value of u and outlet as zeroGradient. Please note the files added to this post. Maybe someone knows how to solve this problem. Best Regards, tH3f0rC3 

April 9, 2011, 01:41 

#2 
Member
Freeman Adane
Join Date: Apr 2010
Posts: 42
Rep Power: 8 
tH3f0rC3,
I am not sure what you meant by "very good". But, please be advised that you might not be able to match the exact solution (experimental or 'analytical") perfectly, unless you're simulating another numerical work with the same problem. Haven't said that, you have to make sure that your problem was setup rightly and there's no user error. I think your 100 iterations for 30m/s...might not have given you converged solution. Try to run it a bit longer say, 500 to see if your solution changed. if it does, extend it further until there's no significant change. If it doesn't, try to extend your outlets further from the region of interest and check your mesh too. Refine the region that might have recirculation flows or drastic change of physics. Note that doing this later one might require different turbulence model beside wall function ke. Lastly, I presumed that you expect only german/nonenglish speakers to respond to your post. The attached files are mostly in nonenglish texts, therefore I couldn't RUN or crosscheck it for you. Is your geometry a tjunction or ? what's the size of your domain, etc....? For the divergence issue, you may want to try the ff: 1. Reduce the time step size (deltaT) 2. Extend the domain with the outlets further downstream 3. consider switching the outlet BC to something different from zeroGradient, such as pressure, inletOulet...(see the OF doc for details). These BCs allow flows to cross the boundary and are more robust and 'stable' than ZG. If you extend the domain, these inflows (if any) are more localised, and its upstream effect on the results are negligible. If none of the above doesn't solve it, then double check your problem setup, especially is your transient and you're solving steady state or vice versa, etc. regards 

April 9, 2011, 07:12 

#3  
Senior Member
Join Date: Mar 2011
Posts: 155
Rep Power: 7 
Hi freemankofi,
with very good I mean, that the velocity doesn't converge. Quote:
There are two inlets (Dueseneintritt and Brennerinlet) and two outlets (Inlet_Outles and Abgasoutlet). All the others are just walls. To your third point: I can't allow that a flow crosses the boundary because there are walls where no flow is allowed to cross. Or didn't I get you right? So which BC you would propose to use for the walls? I want to solve my case steady state as the first step. Later I will try the transient version. But the aim is to get to know the velocity field in the steady state case. For a better understanding of my case I have send you two pictures. In picture 1 and 3 you can see the case. I have added the important names to the geometry. In Brennerinlet hot air flows into the room. On Abgasoutlet the same flow flows out the room. On InletOutlet there is in reality a ventilator which sucks in the air and blows out the air through the Dueseneintrittelements. The Halterungsgestell will be heaten up by the hot air. In reality there is another geometry hold by the Halterungsgestell taht will be heaten up. I have now recognized that it would be better to add in a simple version of that geometry, because now the flow from the little pipes above and below the Halterungsgestell will "collide". I hope you can now understand my case better. Thank you for your advices. I will try on Monday! :) Best Regards, tH3f0rC3 

April 10, 2011, 14:38 

#4 
Member
Freeman Adane
Join Date: Apr 2010
Posts: 42
Rep Power: 8 
tH3f0rC3,
I think you might have a 'fundamental' issue. If your timeline is not a crucial factor, specifically for noncommercial project, I suggest that you approach this problem in more than 1 phase. For phase 1, remove the bottom part (hulterund....) and model only the top part. This will allow you to build much confidence in the setup and all other pertinents that come with it. The subsequent phases you model the complete geometry. I wouldn't put BC at "Abgas..." unless you truly know the exact outlet conditions which isn't the case. Therefore, consider adding about 12D pipe length to it. D is the hole diameter. In this case, this outlet BC effect wouldn't affect your results and might give more stable solution. What's the BC at the right part of the middle section (one with nipples)? Is "Duesenoulet" means "outlet" BC with ZG? I wouldn't go for that. From the picture you sent, it looks that, technically, those nipples are NOT "outlet". Outlet means section of flow domain where the fluid exit. They're just either "distributors" or "suckers" depending on the pressure difference between the inside of the middle box and its bottom. is that correct? Therefore, I'll consider using either "pressure" or "inletOutlet" BCs. In other CFD package you wouldn't need to specify BC for them so far as you defined them as "fluid volumes". Try to solve the flow much longer, say 5001000 (or max residual < 103) depending on the mesh size. Lastly, please double check all your flow conditions including density, viscosity, etc to make sure they're all correct. Try to understand the main problem you're trying to solve and ask all the necessary questions, such: is the correct physics being implemented in the code? is it the same in the 'real life'? Since CFD hasn't reached a stage of using it as a 'blackbox', the user understanding of the problem at hand is VERY crucial of getting the correct solution. If you can send me the image of the computational mesh, that would be great. Make sure that your mesh are also good for specific turbulence model using. A typical ke wall function might only be good for qualitative results since your domain involves curvature effect and probable flow recirculation. See attached my 2D sketch of the problem. The question marks are those you might consider and my suggetsion of the split is those lable "A" and "B". Regards, Freeman 

April 11, 2011, 02:15 

#5  
Senior Member
Join Date: Mar 2011
Posts: 155
Rep Power: 7 
InletOutlet is in this case an outlet. There is a flow going outside the volume. Because I have another case which "starts" exactly there the name InletOutlet is a little bit strange.
It is just the same with "Duesenoutlet". Here a flow comes into the volume. It is just the same flow going ou the volume on InletOutlet. And than there is one inlet (Brennerinlet) and one outlet (Abgasoutlet) left. On the Brennerinlet hot air comes into the volume and on Abgasoulet the air can leave the volume. I have sent you pictures to make the case more clear. Quote:
I didn't get you at the following point: Quote:
Quote:
tH3f0rC3 

April 11, 2011, 10:57 

#6 
Member
Freeman Adane
Join Date: Apr 2010
Posts: 42
Rep Power: 8 
tH3f0rC3,
Sorry I didn't know that "Duesenoutlet" is the same as "InletOutlet". The inletoutlet BC is the same as specifying pressure or "Opening" in CFX. What it does is that it calculates local velocity based on mass conservation using the neighbouring nodes. This means that the velocity can be negative or positive. If you have directed your flows out of the domain (v_out positive) then a negative value will means flow admitted to conserved mass locally. So, the name is not "strange" because it matches its purpose. It is more stable than ZG because ZG is setting respective gradient of the respective parameter to zero and the unknown value is usually computed by the first order. I saw your figures, however, I couldn't figure out which part is the flow domain and which is, say wall. I don't think you anwer my other question, are the nipples (Duesenoutlet) for "naturally" distributing/spreading the flows? That's, what's their purpose? From my 2D sketch, I understand that, the flow enters the middle section duct and somehow expect to go through those nipples (small cylinders). Is that CORRECT? If yes, then you don't need BC at their outlet. Mannually, define the WALL BC and avoid using DEFAULT as wall. In that case, the solver will treat them as flow domain. Remember to include their vertical surfaces in BC wall if you choose this route. On qoute 1: It is not good to put outlet BC "exactly" at the region of interest when one don't know the "exact" conditions. For example, you can't specify outlet BC (zero gradient, ZG) for a laminar pipeflow at length 70 times pipe diameter abd expect to get accuate/good results. First, you're using ZG because you don't know the "exact" conditions at the exit. Note that you're solving for velocities (momentum), pressure gradient(mass conservation) and temperature(energy), and therefore you've to specify their exact values at all the boundaries including the exit of the domain. That's, you need to specify the exit velocity, pressure and temperature. For this just mentioned pipe flow, those values are NOT available unless you used analytical solution which then ridiculous the numerical solution. Therefore, this and many CFD problems, the exit/outlet values are always "NOT KNOWN", they have to be estimated somehow in order to solve the problem. For a laminar pipe flow, you can then assumed that the flow will be fully developed at some length (140 pipe diameters, conservative estimate), hence ZG at the outlet. From the above explanation, unless you're pretty sure that the flow is fully developed at "abs....", then ZG. I am of certain from your geometry pictures sent that using ZG there will not give you good results if you even get a converged solution at all. Nonetheless, if you known the exact exit velocity or pressure values as you've 30m/s for the inlets, then yes, you've to specify them instead of using ZG, inletoutlet, etc. If those are not known, which I think is the case, then you might want to consider my first suggetion. Qoute 2: Decent mesh size. For ke wall function, your y plus value has to be above 25 in order for the turbulence model to be valid. Thus, you've a relative coarse mesh. The down side of this is that, you might miss some of the flow feature such as recirculation zone. kw based model are pretty good at taking advantage of the both coarse and locally refined, with y plus not even much of an issue. You might want to look into that.... You also might want to perform grid independent test (changing the mesh size) to ascertain that your result doesn't depend on the mesh size. I hope these help... Freeman 

April 12, 2011, 02:12 

#7  
Senior Member
Join Date: Mar 2011
Posts: 155
Rep Power: 7 
Hi,
thanks for your answer. It helped a lot! I'm afraid I didn't get you at this point: Quote:
To answer your question: :) Through the small cylinders the flow which left the volume at InletOutlet will enter the volume here again. I'm simulating the flow from InletOutlet to the small cylinders in a seperat case. From this case I know the different values of velocity at every outlet of the small cylinders. And yes, the job of the small cylinders is to distribute/spread the air onto the geometry that shall be heaten up (which lies above the lower small cylinders and under the upper small cylinders). Best Regards, tH3f0rC3 

April 12, 2011, 18:58 

#8 
Member
Freeman Adane
Join Date: Apr 2010
Posts: 42
Rep Power: 8 
Assumed there's a node, np which has neighbours nb and nw as example in 1D flow with nb at the boundary, say outlet.
nwnpnb nw and np are not known with nb supposes to be known because it's at the boundary. If it's known, great! But usually, it's NOT! So, for using ZG, nb = np which means that there's ONLY 2 unknowns instead of 3. Using "InletOulet" or "OuletInlet" or "Pressure", it uses mass conservation: m_w+m_b=0 => m_b=m_w. Knowing the mass, velocity can always be calculated using density and area/volume. Since nb is outlet, it can be taken as negative or positive depending on the sign conversion used (see OpenFOAM manual for it). If it's positive, and the calculated nb was negative, then flow will be admitted to the domain (inflows), and vice versa. So, if you have the exit velocity values, then specify them but check the Openfoam conversion, I am not sure with that but I think positive might be okay. Did you actually measured them or you estimated it from flow rate or mass? Cross check that mass is balanced for your entire domain: mass/flow rate through ALL inlets = mass/flowrates through ALL outlets of the domain. Since a fixed Value gives NO room for the solver to adjust and resulting in instability. Try, if it fails and then give my first suggestion a shot. Send me message anytime if you need additional clarification. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
mesh file for flow over a circular cylinder  Ardalan  Main CFD Forum  6  April 17, 2010 23:40 
how did I see next time step of velocity cotour ?  Andy Chen  FLUENT  2  June 30, 2009 12:48 
DPM UDF particle position using the macro P_POS(p)[i]  dm2747  FLUENT  0  April 17, 2009 01:29 
Convergence moving mesh  lr103476  OpenFOAM Running, Solving & CFD  30  November 19, 2007 15:09 
Variables Definition in CFX Solver 5.6  R P  CFX  2  October 26, 2004 02:13 