Numerical Diffusion in Star and Fluent
 

So I recently worked on a laminar mixing species transport problem in Star. I had done this problem in Fluent before and gotten good results, so I wanted to see how robust star's solver would be. It was a simply Y connection with two similar species. I noticed that, unless I had the mesh aligned with the flow, I got crazy amounts of numerical diffusion. The same problem in Fluent however was handled (similar mesh size and settings, also unstructured) just fine, with almost no noticeable numerical diffusion.

I have three questions:
1. Has anyone experienced this before?
2. Is this a sign that Star's solver might simply be weaker?
3. Does this mean that their solvers for all other equations might fall to the same weakness? I.e. should I be worried about momentum and turbulence models being too diffuse?

This might simply be an issue with the default setting for the calculation of convective fluxes.
Did you really use similar schemes in both solvers?

Numerical diffusion
 

Thanks for your response. To my knowledge the default order for the equation in star is 2nd order. I'll check this today to be sure. I did look through and changed the diffusion model from Schmidt number to an appropriate diffusion coefficient. I using the exact same geometry.

Any other thoughts? I am hopeful there is something silly that I missed and that it doesn't have a ridiculously high numerical diffusion.

I noticed you opened the same thread in the CCM+ subforum.
Are we talking about StarCD or about CCM+ ?

For CCM+ and Fluent, I know for a fact that you can obtain accurate results with good control over the numerical diffusion errors.

ccm+ can read fluent case files. So you can use exactly the same mesh in both codes.

Do you use the same methodology to determine the numerical diffusion in both codes?

I never compared both tools with a methologic approach to cover this specific topic.

But if you really want to do so, I suggest the typical test case for numerical diffusion: the transport of a passive scalar.

Same Mesh
 

Hey Guys, thanks for keeping this alive. I am really hopeful I forgot something silly and that CCM doesnt lag behind fluent this noticeably.

Yes, I was referring to CCM+. Sorry about that, I forgot that they have two.

The test I am doing is a simple Y junction with species transport, which I assume is similar to the passive scalar. I have posted two pictures. Both use the same mesh, and have the same fluid properties. To my knowledge, the species transport is 2nd order on both. I have turned the diffusion down to 1e-30, so any mixing seen should be numerical error.

I will attach images showing the results from both Fluent and CCM. While in this case it looks like the numerical diffusion is maybe double in Star CCM, I have a more complicated geometry that I have been working with and it is much more noticeable.

Do you think there is anythign else worth investigating? Gradients or settings or whatnot? I noticed when I made a poly mesh in this geometry the diffusion seemed almost worse. Only when I did a trim mesh asigned with the flow did it give reasonable results.

Thoughts? Thanks in advance for the conversation

second order means nothing... you can have a central second order as well as an upwind second order...check the exact scheme you are using in time and space

Set the gradient method to "Green-Gauss" and the gradient limiter method to "Modified Venkatakrishnan".

Thanks again for the comments and suggestions.

I looked into the order of the schemes. In fluent it is a 2nd order upwind. But CCM+ doesnt really state which kind it is. I looked into their documentation regarding the segregated species solver but I didnt see any mention. A bit odd.

I tried changing the suggested gradients, but it didnt make much of a change. I fined the Fluent grid to get an idea of how a finer mesh would help. You can see the attached results. I used the same grid for CCM+. I show results for the default and altered gradient methods.

When I talked to a support engineer, they kinda glossed over this fact and said to try a different trim grid. Sure that works, but I will not always be able to have a grid aligned with the flow, so I do not consider that to be a sufficient answer to this problem.

Any final thoughts as to what else to try? I have 2 more days on my trial license. As always, thanks for all and every idea. I appreciate them.

In Fluent you can set the centred second order scheme, avoiding numerical diffusion produced by the upwind discretization

Good to know. Thanks. I don't know of any way to do that in ccm+

@MachZero

I used a temperature test case and the alternative gradient settings improved the solution quite a lot.

Now when using a passive scalar test case the original setup seems to produce slightly better results. Which is what we can also see from your pictures.

But the most impressing result we get by switching between first and second order ;-)

Yeah. For comparison I switched to first order (secretly hoping they accidentally
Mislabeled the methods) and it was starkly different. Still surprising how different it was from fluent a results

Interesting thread and question. How is the velocity field behaving? Could it have an impact on the scalar diffusion?

Fluent & Star-CCM+ both uses limiters. The difference may be in the impact of these limiters and implementation of the convective schemes.

You can try the "Use TVB Gradient Limiting" and also increase the "Acceptable Field Variation (Factor)" to 0.1

This reduced the numerical diffusion at my passiv scala based test case.

Consider that you also have rhie-chow and pressure interpolation which also affects the velocity field. I don't think you can be sure of the settings of both codes unless you have definitive information from the manuals. I'm sure about Fluent, while this doesn't seem to be the case for Star.

Also, how are boundary conditions at wall treated in the two solvers?

It is quite obvious, tough, that if the codes were identical you would have obtained the exact same results. There is certainly something different

License run out
 

Thanks for the replies. My trial license has run out so I can therefore no longer run these tests. During the trial I ran a variety of tests with fluent and star ccm including low re flow over an ellipse, turbulent flow over a cylinder, and micro fluidic mixing. I was unable to get the low re ellipse drag to be within 40% of experiment (40% low). I was unable to get transient averaged cylinder cd to match within 35% (too high). I worked with an engineer from ccm on those so I assume they have been done correctly.

The concern for me is this numerical diffusion issue. Assuming it isn't a simple setting that needs to be handled, more complex micro fluidic problems show very large diffusion based issues. My question is, should I be concerned with the accuracy and numerical diffusion of this code elsewhere (I.e. In other transport equations)? The differences I am seeing with species transport are simply concerning

the problem is not simple...the key of your question is: does the numerical viscosity overwhelms the molecular one in such a way to affect in a relevant way the solution?

The analsysis and the answer depends on a) the type of scheme b) the flow problem.
Laminar flows do not suffer so much but if you want simulate transitional and turbulent flows then the numerical viscosity must be reduced by using high order low-artificial-viscosity discretizations. On the other hand, turbulent flows simulated with statistical models (such as RANS) have solution where the model overwhelms also the numerical viscosity and this problem is less relevant also using low order discretizations.

Have you solved this problem?