Learning Forum

[grayg34]

I am trying to import a solution field into Fluent from STAR-CCM+. My goal is to run a transient scalar transport simulation with a uds equation in Fluent on a fixed steady-state flow solution I have already obstained in STAR-CCM+ . I am trying to avoid resolving the primary flow solution in Fluent because the primary flow solution has some custom models in STAR-CCM+ that would require a fair bit of time and effort to set up. 

I have successfully transfered over my mesh to Fluent. I have written my solution field from STAR-CCM+ to a csv file which I have reformatted and read into Fluent as a point data profile. I then specify the profile data to the respective solution field in the fixed values tab of the region.  

I then initialize the solution. After initializing, I display a contour of the velocity field to check the values it shows zero (the initial condition).

I run the flow solver to compute the face fluxes. I display the velocity contour again, it is now showing the correct velocity field profile data. I checked the steady state mass balance of the flow (it is a cavity with one inlet and one outlet). The outlet is off by about 5% of the inlet. The mass balance does not improve with subsequent iterations. 

Is this the right way of going about doing this? I have not used 'fixed values' in Fluent before but it is my understanding that the solver should calculate conservative fluxes  from the fixed velocity. 

 

[Rob]

If you're fixing (via the profile) the flow field I'd expect some flux balance issues due to how data is stored, transferred and calculated. The amount of difference is very likely model and material property related, and as I've never tried what you're doing (I'd have used Fluent rather than another code) I don't have anything to compare with. 

Once you've got the first iteration or few done you can use Solve>Controls>Equations to turn off the flow equations as you only need to solver the scalar: the remainder of the flow is fixed by the profile. That'll speed up the scalar calculation. 

Overall I can't give detailed advice, and would be checking results very carefully having transferred data in that way. 

[grayg34]

Okay, it is a bit of a long story as to how I got into this situation with the primary flow solution generated in another code... definetly not ideal. 

I have been doing tests of the scalar transport part of the problem with a simplified version of the flow generated in Fluent so I was aware of turning off the equations. That portion of the work is going well. 

Both codes are cell-centered. My csv file of point data profile has all the flow variables at cell centers for the entire mesh.

Working with a simple test problem, constant property single phase turbulent flow in a cavity. I examined the difference between the imported fixed value velocity solution and the flow solution obtained directly in Fluent. The difference is most significant at the wall suggesting to me there are some differences being caused by the turbulence model but it is not clear to me how that would effect the mass concervation  of the fixed value flow?   

If my entire velocity and turbulence fields are fixed is fluent not just solving the pressure equation to calculate the flux? and would that not just depend on density? I would expect the momentum to not balance if the turbulent viscosity differed due to differences in turbulence modeling but I'm not sure how that would effect mass conservation. 

 

[Rob]

I'll not ask....  I also have a fairly limited quota of sarcastic comments before the Forum managers grumble! 

We're assuming that whatever was written out of the other code was the same value that Fluent was expecting, and that nothing is conflicting re wall functions, gradient schemes etc.  Scalar flux will depend on density, diffusivity and potentially some of the turbulent values depending on the flow field and geometry. 

I'm a little stuck with this one as we're heading into specialist knowledge and guidance which I'm not permitted to do as the Forum is public. 

[grayg34]

Well I appreciate any assistance on the manner. Worst case if I have to resolve the primary flow in Fluent I can now use the imported fields as initial conditions which will save some computing time at least. 

I performed a test to confirm my thinking. With the velocity field and turbulence field fixed I changed the material properties: 

• When I varied densitry the outlet flow rate changed. This was obviously to be expected. The sum of the built-in mass imbalance field was proportional to change in density which is also not surprising as the magnitude of mass fluxes changes.
• When I changed the viscosity there was no effect on the mass imbalance or outlet flow rate. This is consistent with my understanding of solving the pressure equation to calculate mass flux at faces.

I have double checked that I have the same density specified in both simulations. My simplified test case has a velocity inlet and a pressure outlet, the global mass conservation should not depend on density. 

The exmples of using fixed values in the fluent user manual suggest you can assign experimentally obtained velocity fields to a region of your simulation. How does Fluent calculate conservative mass fluxes in that instance? The experimentally measured velocities are likely not going to line up with cell centers. The main difference I see between my situation and the given examples is I am fixing the entire field opposed to a small region.

 

[Rob]

If you mean the FIX cell condition you set whatever values you want, and Fluent will try and resolve the gradients etc. If the values are sensible the solver will generally give a good result albeit with some convergence issues depending on the mesh etc. As those convergence issue worsen so too does mass conservation. 

Are you using fluid mass or scalar mass in the above check? The latter don't have a density so rely on the fluid properties. 

[grayg34]

Yes I am refering to FIX cell condition. It seems there isn't much that can be done about the result that it produces?

I am refering to fluid mass. I have not tried to run the scalar simulation with the flow field generated from the fixed value cell condition. If the primary flow fluid mass conservation is not good the scalar cannot be expected to have good scalar mass conservation, hence I am focusing on the primary flow for now. 

I am now also considering a new stratedgy of running the simulation with the flow equation active for one very small timestep rather than the fixed cell condition. I rather have a small change in the primary flow but good mass conservation than a perfect match of the nodal vecity field and poor conservation. 

[Rob]

No, FIX is an older method to force flow in cell zones. It's good for things like jet fans but I'd not recommend setting the whole domain like that.