2D Problem of External flow over an obstruction
I am doing a 2d simulation in CFX.
The sketch is created in x-y plane DM, and then extruded 1 cell thickness (1mm ) in the z direction.
The sketch is a rectangle of length 800 mm and width 400mm
In the Mesher, I have gone for a ‘Sweepable’ method, selecting the source and target faces as the ones across the 1 mm thickness and kept the no. of divisions as 1 , in the thickness direction.
Mesh sizing parameters used : Min size 1 mm , Max face size 1 mm , Max size 2 mm
The node count comes around 565000
BC’s are Inlet : ‘Inlet’ at 208 m/s air flow (Air as ideal gas)
Outlet : ‘Outlet’ at 0 psi pressure , flow normal to boundary
[ Ref. Pressure = 1 atm]
Wall : ‘No slip wall’
Freestream : ‘Opening’ at 0psi
Two parallel faces as ‘Symmetry’
Problems faced :
1) I am getting pressure (total pressure) upstream of the obstruction as 30 psi, whereas it should be 18 psi as per the total pressure formula for a given upstream Mach No. (In this case M = 0.6, T = 298K gamma = 1.4.
Also I get pockets of supersonic flow around the obstruction which seems to be quite unphysical in this situation.
2) When I checked the yplus on the walls , it is in the range 200- 800 , is this the cause of the problem (1) mentioned above ?
Is the mesh too coarse for this problem?
Do I need to refine the mesh further and make it much smaller than 1 mm, like making it 0.01 mm?
Thanks & regards
I think your domain is too short and boundary conditions are also not ok. Can you show us the mesh?
How did you select the domain size? From some literature or on your own?
i am afraid i can't show you the mesh .
i have gone for auto mesh and as the domain is sweepable , i am getting almost fully hexa mesh , with cells of side 1 mm as per the sizing.
regarding the domain size , yes i've taken it not too large in order to keep the cell count somewhat on the lower side with the chosen sizing.
Is that the problem or is it the mesh size ?
To me BC's seem to be fine (given as per whats happening physically in the actual problem)
Far is correct, your question is too general for us to help so the best thing we can do is to refer you to the general FAQS: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
If you have confidentiality concerns then just don't show the sensitive bits. I cannot count the times when the forum as straight away spotted a problem after looking at the mesh.
I agree with Far that your domain is too short. In reality the flow would start changing shape before your inlet (it would not have a uniform velocity profile like you have specified that close to the obstruction) Therefore you are forcing it into the obstruction and therefore increasing the pressure. You should be able to mesh that geometry with "perfect" homogeneous hexes by specifying 1mm for body, face, and line sizing, and also including mapped face meshing.
Thanks for your responses.
here's the update from my side :
1.)i have increased the extent of fluid domain around the obstruction and made it 1m upstream of it , 2 m downstream and the farfield kept 1 m away from the obstruction.
2.) meshing : i have gone for an ICEM-CFD like approach in the sense that i have sliced the (0.7 mm extruded fluid) body in such a way as to make the sensitive areas 'sweepable' where i have then hex-meshed using 'biased sweep' in order to have a better resolution near the walls. In some not-so-sensitive regions , i have gone for a somewhat coarser mesh - all hexa everywehere. The node count is about 425000.
3.) i have used k-epsilon model and a scalable wall fn. ( after around 500 iterations i've found the y+ in the range 0 -100 )
4.) the problem is that so far i have not achieved convergence , the values of pressure are varying as the iterations proceed.
5.) i notice recirculation near the 'farfield; boundary which in turn is trying to pull in air from the 'outlet'
is my farfield too near to the obstruction ?
am i using the correct turbulence model (k -epsilon) ? or
should i wait for more iterations ?
can i do something with the 'time-scale' / 'length-scale' if its just a numerical issue ?
could you give any hints based on the above points
Wish you all a Merry X'mas and very happy New Year.
Thanks & regards
All your questions are discussed on the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
i understood all except the following point ,
"Do a test run with the residuals included in the result file. It is likely a small region of the flow has high residuals while the rest is converging. Consider why are the residuals high in that region .."
How to exactly check which region of flow has what kind of residuals ?
What bit don't you understand? How to put the residuals into the results file, or how to get the results out in CFD-Post, or how to interpret the results?
i don't exactly understand the following :
"How to put the residuals into the results file"
and the general idea i wanted to understand :
(i don't know if the above doubt and this one are related)
How to exactly check which region of flow has what kind of residuals ?
In CFX-Pre, when you set the result file there is an option "Output Equation Residuals". This option puts the residuals in the output file.
The reason this is useful is because after you have run for some iterations and the simulation is having problems converging. You view the residuals, and regions of high residuals are regions which are having difficulty converging. It will probably be in a separation, or a region of poor mesh quality or a boundary condition. Once you know where the problem is you can then do something about it.
Pl. find attached two slides , one showing the zoomed-in mesh and the other shows the streamlines.
Run stopped at 700 iterations, not yet satisfied the global convergence criteria.
W. r. t meshing, I have kept the near wall cell height as 0.12 mm.
In DM, the extrusion of the sketch in the z- direction is 0.6 mm, is this okay from the point of view of setting up 2D Mesh? Or could I have gone for any size of the extrusion as long as it is only ONE CELL thick?
The problems are:
1.There is some reversed flow in regions closer to the 'farfield' and 'outlet' boundary (as indicated by the 'blank' regions) and am getting ‘mass imbalance’ in the domain which is around 13%.
What’s the solution for the above problem?
Also, in CFX Post , I am getting ‘absolute pressure’ of 18. 67 psi just upstream on the obstacle (whereas the value of ‘pressure’ is about 4psi , the total pressure is 7 psi at the same location):
Is this the correct value I am reading to compare with my analytical value= 18.74psi
[P_o , calculated for M = 0.6 , p = 101325 Pa (1 atm) , gamma = 1.4]
Two problems are obvious:
1) Your downstream boundary is too close. Need to move it downstream.
2) Your mesh around the obstacle is poor. The transition from the prism layers to the bulk mesh has too big a jump in mesh size.
Other comments can be found here: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
regarding the pressure , which one should i read to know the pressure upstream of the obstacle ..there are 'three' pressures which CFX Post can show :
1. absolute pressure
3. total pressure
i guess i have to use the first one to compare it with the calculated value which is about 18 psi for the given upstream Mach No. of 0.6 , am i right ?
Pressure = static pressure
Total pressure = static pressure + dynamic pressure
Total pressure = absolute total pressure if operating pressure = 0
as per CFX documentation :
p_abs = p_ref + p_static
p_tot = defined as the pressure felt at a point where fluid is momentarily bought to rest (without losses) and its KE gets converted to pressure
i've kept p_ref = 1 atm
i've used the isentropic , compressible flow total pressure calculation for a given 'gamma = 1.4' , 'M_infinity = 0.6 ' and 'p_infinity = 101325 Pa' , so just wanted to read the appropriate 'pressure' in CFX Post to compare ..hence the query.
1.i have pushed the downstream boundary further , now its 4 m away from the obstacle
2. the jump from the BL into the bulk mesh has been reduced , and made 1.2 times
i have run the case and paused at 260 iterations , here's what i observe :
1. the reverse flow is taken care of
2. the recirculation zone just aft of the obstacle is well captured
3. i note that MAX residual in case of V-mom eqn. is 100 times its corrspd. RMS value
4. the global rate of convergence is around 1(varies b/w 0.98 to 1.03 mostly )
5. i note the Location of Peak Residuals in the OUT file as to be lying in the vicinity of the obstacle
my doubts :
1. how to improve the convergence ? ...like should i increase the 'timescale' for the V-momentum eqn. (or all equations) instead of going for Auto Timescale, which is of the order of 1e-05 ? any general ideas for this case ?
2.My residence time is 0.03 sec which i checked by plotting 'Time' on the streamlines, should i used this as 'physical timescale' ?
3. or should i just let the 'Auto Timescale be as it is and instead go for a higher Timescale Factor ?
Thanks & regards
Your questions are discussed in the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
i have tried to play with the timescale - i.e tried to increase it to 'physical timescale' and also tried to increase the local timescale factor, as i understood from the CFX documentation that if the timescale is too small,
(auto timescale being 1e-5 sec in this case) then the transient effects are resolved too well and then this causes problems to converge.
1.what i am getting is 'reversed flow' from the outlet after 20-30 iterations
there is domain mass imbalance of about 19%
2. also i notice that for increased timescale to 0.03 sec (physical timescale, as denoted by the streamline in CFX post) the solver fails
3. the max residual in v momentum eqn. become 100 times of the rms value when i increase the the timescale factor and also when i go for 0.03 sec timescale ,its not only in v momentum , but other equs. also.
i have identified the local regions of problem in residuals being closer to the obstacle , in its wake region
why this reversed flow flow from outlet and also farfield boundaries ?
pl suggest something, should i run a transient case altogether ?
thanks & regards
The FAQ I already linked to describes a good procedure to follow.
I would also have a look at your flow reporting reverse flow in CFD-Post. Does it look physically possible? If yes then you need to move the outlet boundary further downstream. If no then you have a convergence issue and need to follow the comments in the FAQ.
|All times are GMT -4. The time now is 02:03.|