[May19]

Dear all,

I am simulating the transient flow past a cylinder using C-grid mesh with, Laminar,

using different pressure velocity coupling I am only able to get 0.39 as the amplitude of the C-l and C-d is also slightly high, I have used Simple Scheme, with second order of momentum and pressure and Bound Second Order for Time with these settings I am getting C-l as 0.399 for 117K mesh count and 0.389 for 315K mesh count,



With Piso and only neighbor correction C-l 0.391 for 117K and 0.401 for 315K mesh count,

With coupled solver, and flow courant number 2e^7, the results are more or less the same.

Please help me I am working for more than 1 month but only able to get these results with this much accuracy ideally the amplitude of c-l should be 0.3321 and time avg value c-d must be 1.33.

I have referred to one answer on the forum that guy solved the problem related to the overpredicted value, but did not reply back on the forum

Please help me out

Thanks in advance.

[vinerm]

Have you checked for the accuracy of the Reference Values in Fluent? Default values may not be correct for your case. You need to update Velocity, Density, and Area for accurate predictions of coefficients. Secondly, since the simulation is transient, you need to neglect first couple of flow-through times for any average value calculations.

[May19]

dear sir,
I have simulated by refernce value as :
Since it a 2D simulation the and my diameter is 0.025m

Area = 0.025 (equal to diameter 'D')
density = air density in fluent
length = D = 0.025;
Depth = 1m
Velocity = 0.071576;(calculatd from Re formula keeping density and viscosity of air same as fluent data base)

Time step size is 0.01 sec,

I am telling you results after 40sec of iteration I patch the upper half region of the mesh in downstream with y velocity magnitude of 0.03, to make the convergence faster and setup the oscillation early.

Thanks in advance.

[vinerm]

Are the velocity and density used as reference values same as those used as boundary conditions and material property? For flow-through time, look at the average time required by the fluid to go from inlet to outlet based on the velocity at the inlet. If time required is, say, 4 s, then you should neglect data of first 8 s and then take average over next 12-20 s.

[May19]

Yes, density and the velocity are the same in the reference value panel as the BC, can I ask you little more help with the settings in the method PISO with skewness correction off and Neighbour correction set to 1 and skewness-neighbor coupling off.
Least cell-based gradient
Second order for Pressure,
second order upwind for the momentum,
Bound Second order for Time,
residuals convergence criteria set to 10^-7
the time step size is 0.01 sec, Laminar, Velocity inlet BC, pressure outlet at the outlet, and upper and lower are set to periodic.

Please tell are they best suited or any change requires.
Thanks and Regards.

[vinerm]

The difference you are observing may not be due to numerical scheme but I's suggest using either SIMPLE or FSM with Second-Order time instead of bounded second order. Bounded is to be used only if you face convergence difficulties and is less accurate than second-order due to artificial bounds. Sometimes, least-square gradient does not give expected results, so, try with Green-Gauss Node based (not cell based). I am not sure of time-step that you are using because this has to be such that you can resolve the frequency. So, it depends on Strouhal number. Check what is Strouhal number for your case and then use a time-step. It is quite possible that you will require a smaller time-step.

[May19]

Thanks for the reply Dear vinerm,
I must you are the most generous and cooperative person I ever meet on the forum till now.
Thanks for your advice once again I will do the needful, and will reply with the solution, once I found comparable with the experimental results.

Thanks and Regards

[May19]

Dear sir,

I followed your advice and as per your suggestion, I check my strouhal no and decrease my time step size which is now 0.002, also while taking very small time step I increased the velocity to 0.8 m/s and adjusted the density and the viscosity in fluent database such that to make the Re 100, with Simple scheme only I am able to get C_l now as 0.289 at 117K mesh count and 0.291 at 250K mesh count, it not so bad but very good as compared to my previous result but still now the value is slightly under-predicted, I am expecting the parameters to be within 6-8% of experimental results what could be the reason you said the difference could not be because of the numerical schemes, what parameter I am overlooking?

Thanks and Regards.

[vinerm]

So, earlier it was over-prediction and now it is under-prediction. There is another thing that you need to check against the data. Are the material properties same? And another important thing is that some researchers use wetted area or the area up to the angle of attachment for determining the coefficient. You are using full area, which is the common practice but there are some researches who follow uncommon practices of using reduced area. So, if layer separates at an angle of 80, then area to be used gets reduced and coefficient increases. So, check for these two aspects, material data and area for normalization in the experimental data you are comparing against.

[May19]

Hello sir,

I get good results for the lift and drag coefficient by your advice and now results are in 4% error only.

I want to decompose the lift force (max) into, Pressure force (max) and viscous force (max), and correspondingly the lift coefficient (max) to pressure coefficient (max) and viscous coefficient (max).

Now the problem is fluent is not giving the right value through report>forces, it is giving correct answers to drag decomposition but not for lift.

Please help me out.

Thanks in advance

[vinerm]

Are you using correct direction vector for the lift? It should be normal to drag vector, doesn't matter how the body is aligned with respect to the coordinate system. Secondly, major contribution in lift would be pressure and not viscous.

[May19]

Dear Sir,

Your advice worked well and the component problem also resolved, besides your suggestion one problem was also there that fluent uses the last time step value one simulated to obtain the forces and if that particular time step is not of the max lift, pressure lift, and drag lift coefficient then corresponding forces will not be the max one.

Now I want to make one thing more into your notice if you can help me out, for my intuitive study I run the simulation with the PISO scheme and COUPLE scheme both. The results I got for the RE 100 case is matching with the literature I am referring to, by the use of the COUPLE scheme, but the results are slightly (~8%) underpredicted with the PISO scheme.

Hence I adopted the COUPLE scheme for the simple flow past the circular cylinder.

But now I am analyzing the slotted cylinder (a small square cut in the cylinder at AoA of 0 in part of the cylinder directly facing the fluid ) in that the case the COUPLE scheme is giving the lift coefficient almost same as compare to non-slotted case and PISO again giving the value less than COUPLE scheme. DRAG coefficient Time-averaged value is almost the same for both the schemes slight difference in the max amplitude reached for drag.

Please help
Thanks in advance.

[vinerm]

For low flow speeds, Coupled is the only one you can rely upon since the coupling between pressure and velocity field is very tight. However, as the velocity keeps on increasing, on average, this coupling loosens to some extent until the flow becomes supersonic. So, if you working with low Mach number flow and also low Re, use Coupled with pseudo-transient or Coupled with transient.

[May19]

Dear sir,
Since in my case velocity is only 1 m/s^2 and Re 20 & 100, hence couple will be the best from your previous answer and now I can deduce the answer for the same.

For slotted cylinder, one doubt is occurring in my mind that whether I should include the slot part in the cylinder along with the curved surface area to calculate the lift and drag or I should exclude it.
So lift and drag force should be calculated on the circular surface only excluding the slot geometry or including it.

Thanks and Regards

[vinerm]

Force will be calculated over whole geometry, i.e., including the slot if the slot is meshed. However, as far as coefficient is concerned, it does not matter. As long as you specify which area is being used for determining coefficient, it is alright.