Basic Question - Mesh Quality
As part of my final year project I have been asked to produce a technical report which presents the quality of a mesh generated for an applications from a GAMBIT tutorial of my choice, with critique of mesh quality, highlight good and bad areas, and make suggestions for further improvements.
I would like to add I am not trying to cut corners and trying to get you to answer my question just attempting to extend my knowledge. Bare in mind the said tutorials are basic as is my knowledge of CFD at this stage
I am wondering;
What constitutes a sound mesh?
How can I define between good and bad areas?
Are there any generic improvements to increase my mesh's accuracy?
Any brief advanced methods to increase my mesh's accuracy?
Please let me know if there is anything else you require.
I too am very new to CFD, but I might be able to help a little.
A "good" mesh is generally one that, when refined (i.e. made finer) gives the same "answer." Depending on what you're looking at, this can be a variety of things from pressures to flows to heat transfer coefficients.
Another idea of "good" might mean how refined the mesh is in relation to the fluid flowing against a wall. In this case, the y+ dimension is usually used, which relates boundary layer thickness to how fine the mesh is. There are general rules of thumb for various applications. For heat transfer (my field), y+ should be in the range of 1-2.
I'm not a Gambit user, but your question transcends individual software packages.
A good mesh is one that allows you to compute a solution of the desired accuracy in a practical amount of time. You can see the implications of this relatively simple statement.
A "practical" amount of time basically means using as few cells as possible so that your computation doesn't take a month. You can throw a bazillion decently shaped cells at any solver and usually get a somewhat accurate solution.
As soon as you start using less than a bazillion cells you introduce the idea of clustering, or non-uniform distribution of cells. This brings into play a couple factors. If your clustering is non-uniform, have you clustered to where important things are happening and used a coarse grid where not much is going on? And, a non-uniform distribution of points (combined with a geometry of realistic complexity) introduces the concept of cell shape; that non-uniform distribution of points is going to introduce distortion into the cell shapes and that may not be good for the computations.
Finally, "accuracy" of a CFD solution is often poorly defined. Poorly in the sense that you need to know what exactly it is you're trying to compute. Too often people show graphs of pressure coefficient or a contour plot of Mach number and make generally vague statements about how well the results match data theory. You need to know what it is you're trying to compute: drag, wall temperature, the path of a vortex core. Each of these has distinct an unique implications for how you generate the grid.
Now with all the motherhood bullshit out of the way, here are some practical things to consider. They echo some of what puga wrote above.
Look up the topic of Richardson extrapolation. If you double the density of your mesh, does the accuracy of the solution improve? If you have 3 meshes of varying density, how do the solutions on each compare?
Consider looking at the wall spacing using the idea of Y+. Make two grids, but one just has a wall spacing 1/2 or 1/10 the size of the previous. How does that effect the solution.
What difference is made for computing the same solution using two different grid types? For example, compare structured hex to unstructured tet grids of equivalent density.
You can also try to introduce poor cell shapes into a grid to see how that effects the solution. (Afterward, you can compute some cell quality measures like aspect ratio, adjacent cell volume ratio, skewness to try to identify the culprit). In fact, what's a little easier than trying to make a grid better is to take an existing grid for which you have a solution and mess it up somehow. Or, if you're generating structured grids, compare a solution for a grid that's been created using a simple algebraic technique versus one that's been smoothed by an elliptic PDE method.
Finally, there's the whole topic of adaptive meshes in which the non-uniform distribution of points is guided by the flow field - points are clustered where gradients in the solution are high (e.g. shock waves, boundary layers, vorticity). Based on your description of your own experience this may be beyond the scope of this problem, unless Fluent (which I assume you're using) has a simple switch that you can use to turn this on.
I hope this rambling is of some help to you.
I totally agree with John, but since he didn't specifically talk about cell shape, I will add a little to this thread...
You will find lots of metrics for ranking elements by skew or determinant, max angle, volume change, etc. The variety of formulations shows that even advanced CFD analysts are not really sure how to best define quality. In fact, I heard that Fluent developers may be working on a new metric for the next release...
I often think about it in terms of first principles... We have formulas to predict the flow thru very simple perfect "cells" or "elements", but then to fit these cells to complex geometries, Handle volume translation, etc. we end up distorting these cells a little so that they do not match the ideal. Over time, these solvers have become more robust, but the solutions are still not as good with less than perfect elements. (Garbage in => Garbage out)
So, why not strive for perfection? Because of the all mighty dollar and the finite duration of our lifespans. We need to strike a balance between the perfect mesh and getting a relatively accurate solution in the near future.
As computing power gets better, I expect that we may eventually be able to just toss a bazillion perfect tiny elements at the solver and and get the answer back pretty quickly. When that is possible, no one will care about meshing anymore, certainly not manual meshing anyway.
2 quick bits of related anecdotal humor.
I was once working with someone who had severely defeatured his model, removed lots of small holes, replaced fillets and champers with sharp corners, removed ribs, etc. It didn't even resemble anything anymore. I asked him why and he said it was to improve mesh quality (slightly):rolleyes:. I pointed out that he now had a more accurate solution of a model that had nothing to do with what he was investigating. CFD is for a reason, and good geometry capture is worth its cost in element quality (within reason).
Another time, I got a call from a customer who was getting very frustrated. He was using the rarely-used "worst" button, a button in ICEM CFD that finds and highlights the worst element in a model so you can fix it. He said "every time I fix the worst element, there is another one!":confused:. I told him to relax, there is always a "worst" element, but is it good enough (for its location)?
There are some very good materials at
Do you know how can I improve my mesh so as to eliminate a negative volume? I'm doing a mesh of an airfoil of a World Series by Renault car, I've done all the mesh in Gambit but when doing the Grid in Fluent, it says I have a negative minimum volume value and that I have a non-positive volume. I've checked in Gambit the option "Check" (right-click at the info button) and said all volumes are valid. So I don't know where's the negative volume and how to solve this problem.
If u or anyone else knows, please tell me.
Thank u for your help!!:)
I have only gone thru the basic Gambit tutorials and never used it for production work. In ICEM CFD, hexa quality problems always come from badly shaped blocks (fix with move vertex to improve topology), or from bad distribution, Fix the distribution.
For unstructured Tetra/Prism mesh, bad elements usually come from over-constrained geometry. See if you can find where your model has the poor quality. You will probably find elements with 3 or 4 nodes constrained to points or something like that. Do you need those constraints? Are they capturing details you need? Would refining the mesh in that area give the mesh more room so it could improve its quality...
If you can post a pic of the bad quality, I can suggest a better fix.
Or, ask a new question on the forum under the gambit header and a gambit expert may step up. (-mAx- is always good)
Do you know how to post pictures saved in your computer??
My problem is that I've done a Boundary Layer in one face and meshed that face. Then I meshed the volum with a Hex/Cooper scheme taking as a source the face I previously meshed. The thing is that while the cells go from one side (the meshed face) to the opposite side, they skew themselves. Theoretically they should go straight to the other side, but instead have little desviation.
I know this is quite confusing written in words without images, but I've tried to insert images by the button but it's only for internet. I don't know if I can post a saved one. Also, do you know someone who could give me some more advice??
Thanks a lot for your help.
To attach an image... if you reply to thread (not quick reply), you will see a paper-clip in the top row... Click it and attach the image files... Later you can come back and use the pulldown to actually insert the image between the text...
But no, I can't help here. This type of poor quality is specific to Gambit cooper tool. You will need to ask a question on a new thread and maybe a gambit expert like -mAx- will help.
|All times are GMT -4. The time now is 00:12.|