ICEM Tetra mesh, Size reduction and Skewness problem
I am using ICEM to mesh the combustion chamber of a Stirling engine MCHP.
What I am looking for is mainly heat transfer through walls.
Unfortunatelly I cannot show the geometry due to confidentiality issues :(.
What happens basically is that the main combustion chamber is surrounded by two other conical walls which create a path where air gets preheated before entering the main combustion chamber.
So I need to mesh these conical walls to investigate heat conduction in Fluent.
I also need to mesh the cylinder walls to investigate conduction and heat transfer to the stirling engine working gas.
I tried to block it initially but it seemed that it was one of those complex geometries you need to use tetra mesh.
So what I am doing is:
Create a Fluid body for my mixture and solid bodies for each walls I need to mesh;
Assign the mesh size to each surface (small to capture walls of 1mm thickness);
Compute volume mesh (robust octree).
The resulting mesh is two big - >10million cells- and I want to have around 3million maximum.
I understand that meshing all these walls will create more cells so I need to have less cells for the fluid domain but of certain quality.
So when I assign larger sizes I get a fluid domain that looks terrible.
The diagnostics say I have many multiple edges elements which are mainly at the contacts of each part.
I do smoothing but when I import to fluent I get a skewness warning..
In the solutions I cannot reach convergence, mainly in the turbulence residuals , k and ε which fluctuate around 10^-1 values.
I know am missing something but how can I obtain a smaller mesh of good quality with tetra?
Apologies for the huge thread and the lack of visual content.
All the best
For CHT, I sometimes just mesh the CFD portion and then extrude the surface mesh to create the solid region around it. I am not sure if that would work for you, but it does save a lot of mesh because you can be much more efficient with an extruded mesh thru the thickness and not need to mesh so fine along the surface.
Sorry, it is tough to help more without at least a sketch or zoomed in image of your problem mesh. I don't think either of those would give away important features of your design, but it is up to you.
thaks for your reply.
Mesh extusion is a bright idea but i couldn't get it to work.
I have, say, a conical wall imersed in fluid so there is surface mesh in both sides of that wall. I messed a bit with extrude mesh but could not get anything.
I read through some of your tetra related posts where you wrote that one can use the octree tetra, delete the volume mesh, laplace smooth the surface mesh and use a volume filler like TGrid to mesh the domain.
This opened new possibilities for me as I can control the mesh size by the expansion ratio and I already have a skewness issue when I read in to fluent. I think TGrid is programmed to overcome such issues.
The problem I am facing though is that although I enable the flood fill application (TGrid with many material points) the volume mesh is not assigned to the different solids so when I import to fluent I have only one volume domain containing both the fluid and the solid regions. This way I cannot assign different materials to the solids in fluent.
Is there a way to get around this?
In the compute mesh tab I set volume part to inherited and compute from existing mesh.
I guess there is something wrong with my settings..
I understand that lack of visual content makes it difficult and boring for you to help and I so want to diplay something but my supervisor is very strict about it, sorry..
Thank you very much,
When you say "use TGrid", I assume you mean using the Delaunay TGLib algorithm in ICEM CFD... If you are using a version (such as 12.0) that has both "TGrid" and "Delaunay with TGlib/AF", use the Delaunay option. It is has a much better hook-up.
As I understand it, the fill is working for you, but you want it to use your material points to assign solid and fluid regions...
You can have it do this automatically by turning on the material points option under the Global Params for this mesher.
If you already have the mesh generated, you can still use the flood fill from ICEM CFD. Just go to Edit Mesh => Repair => And find the option called "Flood Fill". It looks like a paint can spilling.
Click that and it will find the material points in the model and assign the element containing that point to that material. Then it assigns all the volume elements connected to that element, and then all the elements connected to those elements, and so on until it is surrounded by shell elements.
If you have two elements within that volume, it may report leakage.
Once elements are in specific parts, it is easy to assign different properties in Fluent (or other solvers).
Hi again Simon.
I have been playing with flood fill and strangely the flood fill function set up in TGrid reports an error but if i run it from edit mesh it works fine and makes the material assignment.
Still I could not reduce the mesh size considerably but the import to fluent looks a bit better.
About delaunay with tglib and af i could not find it in my settings.
A video in the utube channel using this approach was on ICEM CFD 12.1 version and I am using 12.0.1.
Is this why I cannot find it or do I need first to enable something in the previous steps?
and given that there is not such option, what would you recommend as the next best approach?
Is it plain quick delaunay or should i stick with TGrid with AF?
Thank you very much
Small progress & some visual
By messing with the part sizes I managed to improve my octree mesh, create prisms and even some nice hex elements.
Fluent however liked my TGrid mesh better so I am sticking with it for the moment.
One thing that happens and causes problems to my imports in fluent is some tri elements that do not respect their surface and some holes in the surface mesh.
I have attached a picture where there is such a hole and I pointed an element which is off the surface by some angle.
In the second picture I pointed some more of those elements from a different part.
There I zoomed on some fins and it seems like the "turned" elements on one fin jumped from the adjacent fin..
When I import to fluent, it separates those elements from their origin
and the created zones mesh up my bocos.. Of course, I could not merge them in fluent..
Is it possible to fix that locally in ICEM 12 without re-meshing everything?
Again, thanks a lot!
All the best
Better late than never?
Yes, this happens with the Octree mesher because of your particular combination of mesh size and edge criterion relative to the geometry feature size... Those nodes just don't end up on the right surface.
You could prevent these with adjusted settings, but once your mesh is generated, if you don't have too many, the mesh editing tools can be used to fix these pretty quickly. I would try to merge the nodes. Select the node on the surface first, then the node of the peak. It will collapse down.
As for TGLib, yes, it was added at 12.1. Earlier versions had a somewhat crude TGRID hookup that was not as good as the standard Delaunay hookup.
|All times are GMT -4. The time now is 05:01.|