Learning Forum

[robert reis]

Hi Friends,

I have an issue with the mesh refinement in the water tight workflow and was hoping someone could give me some guidance.

I have a simple structure made up of vertical and horizontal plates - see P1.  The windward plates have holes in this version.

I have all of the faces named so I can control the face size on each plate using the local facesize tool. I have different sizing on the faces and edges of the vertical plates compared to the horizontal plates.  The intention is to have a finer mesh around the corners of the vertical plates causing separation, coarser on the horizontal faces.

Where the vertical plates meet the horizontal plates there is an automatic mesh refinement of the corner zone as expected - see P2. The view here is underside of top horizontal plate.

The problem I have is that this refinement is reflected onto the top surface of the upper plate - see P3.

One issue with this is it increases the overall mesh size for the problem - especially when inflation layers are added.

However my main concern is the transition between the coarse mesh to fine then back again along the top flow surface - the mesh does not look good, which makes me concerned about quality of simualtion. - See P4, P5 and P6. I have used poly-hexcore.

Does anyone have a suggestion how I can fix this so that the top face has consistent larger size alomng full length (with exception of edge transition zones?)

Thanks

 

 

 

 

[Rob]

What are the purpose of the support struts? The refinement is a result of the geometry, and I'll also point out the lack of refinement (as a comparison) on the yellow strut. 

[robert reis]

Hi Rob,

Thanks for taking the time to have a look at this.  You have asked 2 very good questions which I think will help me understand bigger picture.

I have purposely set the face size of the yellow strut in this example to the same as the horizontal plates.  As noted there is minimal refinement compared to the opposite end.  I am fine with this in principle - the flow is from left to right.  There is separation at left side and for the velocities I am looking at the flow does not re-attach at right. But as you say the refinemement is a result of the settings on the struts.

Secondly, the analysis is intended to parametrically look at the force on the struts for various size openings (solidity of strut). I was thinking of it this way - the force on the horizontal plates in almost a "constant", and not of large concern.  Yes there will be some boundary layer variation due to the recirculation between upper and lower plates due to solidity of the struts and resulting velocities, but I thought I could go coarser on the face sizing for the horizontals compared the verticals which will influence result more.  Where the struts intersect the horizontals is perfectly as expected with the refinement at the corner.  The issue the top most plate with the reflected refinement which I think is not required.

To add, in order to test my concern I have been running a grid independence study varying the face sizing of the vertical and horizontal plates,  but keeping rest of domain constant.  I have been using total force in X-direction as the dependent variable.  As I decrease the face size the total force increases, up to a point and then it begins to reduce.  For example see below - horizontal axis is cell count and vertical is total force.

So I'm thinking thios is pretty weird and needed to find an explanation.  Are we seeing a variation in force due to the refinement of the top face cells?  As we go to 4M cells, the top face becomes more consistent and uniform rather than banded as shown in my pics above which are from the 1.5M cell version.

What I need to do is re-run the simulations to capture the X-force component of just the top plate to see how that varies with the mesh issues above.

However if I could isolate that top face from the mesh refinement of the struts below and not have the banding would be awesome.

Happy for your thoughts?

 

[Rob]

The top plate refinement may be the result of the proximity size function. Can you check what surfaces are present and whether you need to rethink how the struts attach? You may always see some effect unless you turn off proximity and rely more on the local sizing. 

If you retained the data (always a good idea) you can check any results you missed for a steady flow - that's one of the many benefits of CFD! 

If you're seeing a drop in the force like in the plot look for changes in the flow. Numerical values are very "experimental" but you've also got velocity, pressure, turbulence etc in every single cell: there's a reason we spent a long time working on Fluent's ability to print pretty pictures! :) 

[robert reis]

Thanks Rob, Some good points to look at and I will work through.

I am running the sims on a HPC remotely and just noticed in the transcripts I am getting turbulent viscosity ratio limit warnings.  At this stage I am using kW-SST steady while figuring out this mesh strategy.  I figure I'll have a look at the result files and mark the limiting cells and see what the go there is.

In the meantime two final questions:

1. you mention "turning off" proximity - how do you do that in watertight workflow?
2. There may be a simple answer to this and I just missed the important episode in season 1.... is there a way I can "separate" the vertical from horizontal as you mention?

Have a great day.

[Rob]

When you're going through the workflow there should be an option for the size functions in Generate Surface Mesh. You may want to turn off proximity. 

The surface you're meshing come from CAD. How does that look before you go into Fluent? However, if you're turning off the proximity sizing that may not matter. 

[robert reis]

Rob,

Hmmm.... this is what I have.  Options are Proximity, Curvature or Curvature + Proximity.... but no off button.

This is 2023R2 Academic.

 

[Rob]

Try just curvature then - I don't think you have any! You're then reliant on the local and surface mesh sizes. 

[robert reis]

Found an ANSYS support ticket talking about going behind the workflow and turning off proximity... I'll give that a go.https://ansys13.ansys.com/KnowledgeArticles/Phase-1/2063807/2063807.pdf