[ceanwang]

Hi,

I am simulating a flow around a 10m x 10m x 3m box on ground at ma=0.1.

The calculation is converging, but the cl and cd value always at -10000.0. I am using the cfg file from euler/crm testcase. Just wondering what I need to change to get the cl value right？is it something about reference length？

Regards,

Cean

[pcg]

Hi Cean,

Check if these two options have the correct boundary names:
MARKER_PLOTTING= ( fuselage , Wing , HTP )
MARKER_MONITORING= ( fuselage , Wing , HTP )

Regards,
Pedro

[Sprotte]

Hi,

just wanted to let you know that -10000 (or 10000) are the default output values whenever the ones obtained in your simulation are smaller or bigger than that. Did you change the reference length?

[hlk]

Hello
Thanks for your interest in SU2
As a previous poster mentioned, the -10000 value is a default max-out value.
This usually indicates that the solution has diverged - Sprotte, when you say that it was converged do you mean that the residuals (output as their log10 value) have reduced by some number of orders of magnitude, or do you mean that the Cl reaches a constant value?
The former is recommended as a more reliable measure of whether the simulation has converged. Given the -10000 output, even if the residual magnitude is reduced I suspect that it is not really converged.

I suggest using a lower CFL number and using CFL adaptation (if you were using CFL adaptation before, check what CFL number was output somewhere before the Cl blew up, and then use a constant CFL that's less than that).

Given your Mach number, it would also be a good idea to check that you are using an incompressible simulation. (Mixing cases where the density gradient is physically near zero with simulations that rely on accurate computation of density gradients tends not to work out very well (: )

[ceanwang]

Originally Posted by pcg

Hi Cean,

Check if these two options have the correct boundary names:
MARKER_PLOTTING= ( fuselage , Wing , HTP )
MARKER_MONITORING= ( fuselage , Wing , HTP )

Regards,
Pedro

These two settings are right.I only have Wall and Farfield conditions.

I have "Non-physical points" first, and found out some boundary value are wrongly set. Maybe still some faces have wrong value. I'll check.

[ceanwang]

Originally Posted by Sprotte

Hi,

just wanted to let you know that -10000 (or 10000) are the default output values whenever the ones obtained in your simulation are smaller or bigger than that. Did you change the reference length?

no. still = 1 I think.

[ceanwang]

Originally Posted by hlk

Hello
Thanks for your interest in SU2
As a previous poster mentioned, the -10000 value is a default max-out value.
This usually indicates that the solution has diverged - Sprotte, when you say that it was converged do you mean that the residuals (output as their log10 value) have reduced by some number of orders of magnitude, or do you mean that the Cl reaches a constant value?
The former is recommended as a more reliable measure of whether the simulation has converged. Given the -10000 output, even if the residual magnitude is reduced I suspect that it is not really converged.

I suggest using a lower CFL number and using CFL adaptation (if you were using CFL adaptation before, check what CFL number was output somewhere before the Cl blew up, and then use a constant CFL that's less than that).

Given your Mach number, it would also be a good idea to check that you are using an incompressible simulation. (Mixing cases where the density gradient is physically near zero with simulations that rely on accurate computation of density gradients tends not to work out very well (: )

The residual reaches -3 and still going down. I stopped.

I am using Euler, Direct. CFl =5. the Cl = -10000.0 from the first calculation.

[ceanwang]

just uploaded a screen shot.

[pcg]

The reference factor is usually not 0. Can you upload the configuration file and the screen output?

[ceanwang]

Originally Posted by pcg

The reference factor is usually not 0. Can you upload the configuration file and the screen output?

I also want to try the cfg file from testcases\incomp euler\naca0012.

this zip file also includes gmsh's geo file which could generate the su2 mesh.

screen output at #1

[pcg]

I generated a coarse mesh for your geometry, literally clicked buttons on gmsh until something came out because I never used it before .
It seems to be just a matter of increasing the reference area, the geometry is huge so it makes sense. At 10000 m^2 I started to get numbers.

Based on my personal experience with SU2 I suggest the following:
LINEAR_SOLVER= BCGSTAB
LINEAR_SOLVER_PREC= ILU
LINEAR_SOLVER_ERROR= 1E-2
LINEAR_SOLVER_ITER= 100
MGLEVEL= 2 or 3
MGCYCLE= V_CYCLE
MG_DAMP_RESTRICTION= 0.75
MG_DAMP_PROLONGATION= 0.75

With the above I can usually run at CFL_NUMBER= 10 to 15

Cheers,
Pedro

[ceanwang]

The ground area is 1800 m^2, and need 10000 m^2 to ref as your test.

What's the ref length and area means?.

[ceanwang]

Changed the ref area=10000.

Finished after 2402 steps.

Res=-5 but CL=7000.

Screen shot uploaded.

[pcg]

Your geometry is 60 kilometres in the x direction. Make sure to use meters if you are using SU2 with SI units.
Reference area and length are part of of what goes in the denominator of the force and moment coefficients:
https://en.wikipedia.org/wiki/Pitching_moment
https://en.wikipedia.org/wiki/Drag_coefficient
https://en.wikipedia.org/wiki/Lift_coefficient

[ceanwang]

i used mm. no wonder its so big.

thanks.