[Jon Faried]

Hi, everyone!

I'm currently trying to validate the benchmark DARPA Suboff (submarine) case using STAR-CCM+, and am at a loss as to why I haven't been able to get the residuals to converge properly and for the results to come out correctly. Any insight would be appreciated.

And now for the details...

The mesh is a simple axi-symmetric one (only the bare hull of the sub is currently being tested, no fins and rudders) with a y+ equaling roughly 1, with the axes removed and replaced with H-meshes. I'm afraid I don't have any photos currently handy, but the completed mesh looks like a dome (or half a sphere).

I've managed to successfully run the exact same mesh on ANSYS CFX and obtained excellent results, so I don't think the mesh is the problem, unless there's something about meshes that requires special treatment in STAR-CCM+, in which case I'd value your input.

The submarine has no angle of attack, and is exposed to a constant flow with a Reynold's number of 14,000,000. The mesh is split into four main boundaries: the hull (no-slip wall), the symmetry plane (only half of the axisymmetric mesh is necessary), an inflow section (half of the dome, where the fluid comes in with a constant velocity), and an pressure outlet section (backflow direction is extrapolated; pressure is static, though 'environmental' was tried as well).

I'm currently using the segregated flow model (RANS, K-Omega SST, Liquid). The turbulence residuals are fine (quickly reaching E-8) whereas the mass and momentum residuals drop quite slowly (down to E-3, couple thousand iterations) before eventually (approx. 70000 iters) jumping back up to E-1 and staying put. One way or another, for a simple case like this one I'd expect a fairly quick convergence, so something seems definitely off here.

The pressure and velocity results seem to be OK throughout the entire process, whereas the turbulent viscosity eventually goes haywire and produces wrong results. The coefficient of drag completely misses the mark as well.

I've tried running the laminar case in order to see if turbulent viscosity was the problem, but the case completely diverges. Trying the Coupled Flow solver doesn't work either - it too diverges (even for relatively low Courant numbers).

I get the feeling that I'm missing something trivial here... any help would be most appreciated, and I'd be happy to give more details if necessary. Thanks in advance!

[me3840]

You have a dome but you are using velocity and pressure conditions? That's probably the issue. You will have velocity traveling tangent to its face at some point connecting to a cell with zero gradient and a pressure specified. That's just a nightmare. I would switch your domain to be a cylinder instead.

[Jon Faried]

Originally Posted by me3840

You have a dome but you are using velocity and pressure conditions? That's probably the issue. You will have velocity traveling tangent to its face at some point connecting to a cell with zero gradient and a pressure specified. That's just a nightmare. I would switch your domain to be a cylinder instead.

Thanks for the reply!

While what you're saying certainly makes sense, I get the feeling that this isn't the issue at hand, since:

A. The same mesh (boundary conditions included) was tried using CFX and another solver, and the results in both cases were accurate. Is there a fundamental difference that you know about between the way CFX and STAR-CCM+ treat boundary conditions? (or in general, for that matter?)

B. What's more, the velocity and pressure solutions seemed to be quite accurate, even when the residuals jumped from E-3 to E-1. There certainly wasn't anything amiss at the interface between the two dome shaped boundaries (inlet-outlet), I checked that area.

Have you ever encountered a particular mesh which one solver tackled effectively whereas STAR-CCM+ had difficulty with it? If so, I'd love to hear about it, perhaps I can glean a bit of info that'll be practical in this case.

Again, thank you for providing your two cents, much appreciated.

Sent from my A0001 using CFD Online Forum mobile app

[me3840]

Originally Posted by Jon Faried

Thanks for the reply!

A. The same mesh (boundary conditions included) was tried using CFX and another solver, and the results in both cases were accurate. Is there a fundamental difference that you know about between the way CFX and STAR-CCM+ treat boundary conditions? (or in general, for that matter?)

B. What's more, the velocity and pressure solutions seemed to be quite accurate, even when the residuals jumped from E-3 to E-1. There certainly wasn't anything amiss at the interface between the two dome shaped boundaries (inlet-outlet), I checked that area.

A. Yes, I've seen this many times. There's lots of "stuff" that happens behind every commercial code which makes BCs and discretization schemes that look the same act differently. If something is theoretically a poor idea but "just works" in a commercial code, it's often because the code is designed to help people who don't follow best practices.

B. Define accurate here? Remember the residual itself is only a measure of relative error. Perhaps your initial solution is very good? Perhaps your mesh is coarse enough to diffuse the physics in a location to give a stable but poorly converged solution? Have you looked at the unnormalized residuals? They could be quite low while the relative residual does not converge well.

I'm surprised you don't see any issues in that area, perhaps that means I don't understand how the domain is set up after all, a picture may help. In STAR-CCM+ you can use the 'temporary storage' option on the solver to enable you to view the residuals as a function of space, I would recommend you do that here to see where the largest residuals are.