ICEM mesh problems for sinusoidal leading edge wing
 

Hi everyone.

Ive only just started using ICEM (like 2 days ago) and have been trying to mesh a 3d wing with leading edge tubercles in ICEM. Essentially what I did was follow the 2D wing tutorial that everyone generally gets pointed to, and made it 3D with multiple blocks in the spanwise direction (someone suggested to do it this one on someone elses thread)

My problem is, that while my mesh looks okay superficially (kinda), when I run error checks it comes up with lots of errors, and weird stuff keeps happening when I try to import it into CFX. For instance my boundary conditions all change and become weird, and there are random floating blocks in domain.

Does anyone have any idea what is going on, or what I have done wrong? I know the mesh is not particularly pretty too, but I have been really trying just to get it to work.

If anyone could help me out and point me in the right direction, that would be great.

Here are my files. (both zip files have the same mesh, tubercle_mesh_1b just has the hex mesh. Figured I would give both so you did have to dl such a big file if you have slow internet speeds)

https://www.dropbox.com/s/7zpgq4ink8...le_mesh_1a.zip

https://www.dropbox.com/s/e30u7pzklr...le_mesh_1b.zip


Ans some pics of my mesh, and what is happening when I import it into ansys.


If anyone could help me out and point me in the right direction, that would be great.

Your spanwise edges near the leading edge (on both sides) are associated to the leading edge curve. Delete these associations and try again. If you want to associate to the leading edge, create another split.

That seemed to do the trick more or less, but I am still getting a couple of bad elements that are being weird and seem to be connected to the inlet and outlets (see pic)

I will do a whole pile of smoothing later, but it seems that it isnt set up well enough to start with and smoothing will just mask the poor quality a bit.

So does anyone have any advice on how to refine the mesh on the wing to capture the curvature better with out increasing the node count dramatically?

https://www.dropbox.com/s/7zpgq4ink8...le_mesh_1a.zip

Im thinking that I have done something wrong in the end section.

The first pic is coloured by connectivity, and the second picture shows that the blocks seem uneven at the ends, but I cant figure out if it is actually the problem or how to fix it.

Any thoughts?

https://www.dropbox.com/s/7zpgq4ink8...le_mesh_1a.zip

did you assoc. all faces and surfaces on the wing? try to highlight them by blocking-->faces-->"right click"-projected .. now you should see all blockfaces by color and name if not... do the assoc. and try again.

Matthias, I would refrain from associating faces unless absolutely needed. Unless there are internal faces, or faces close to each other (and the surface mesh is snapping to the wrong face), you do not need to do face associations. I think by making unneeded associations, you can over complicate the model, and sometimes it causes strange behavior if you modify the topology downstream.

Interested to see what you think though?

there is a point..yes. i was pointing that out because of the fact that at the outermost face the wingsurface is probably crossing the blockfaces. so projecting the faces would be my first try. btw. there is a premesh blocking option "project to faces" instead of "project to edges". maybe this would help correctly mapping the wingtip.

Hey Stuart junior

Some changes in geometry and blocking as usual :D as the blocking shown in Simon's tutorial was for sharp trailing edge wing/airfoil. Domain is changed to rectangle. Few curves were constructed to ease the blocking/association. See attached files.


https://dl.dropbox.com/u/68746918/si...alwing_Far.zip

I did attempt to find these and give them a try, but I didnt have much success. I am still learning ICEM so my knowledge is less than extensive haha.

Thanks for that Far, that mesh seems too work quite well. I am still learning ICEM so I was wondering if you could quickly step me through what you did for that. So do you not need all the blocks in the spanwise direction to capture the curvature?

Ultimately I want to make a script for it so I can put various wings in (with different leading edge profiles) at different angles of attack easily. And the way you meshed it seems to work quite well.

I have tried to copy the method Far used closely as I could and I think I have gotton reasonably close considering (see pic1 and 2) but I am still having a few problems.

The mesh is still reasonably nice but I am still getting a few anomalies in ansys where I think there are stray elements or something.

1- In pic 3 you can see an arrow. This arrow seems to be associated with the inlet somehow and im not really sure why (same thing happens with outlet to but arrow points in the opposite direction.)

2 - I cant figure out how to get the boundary conditions to be smooth in Ansys rather than clumping up where the mesh is more dense like you can see in pic 4.

Any thoughts on these issues?

Here are the most recent files if anyone wants a look to see what I may have done wrong, or see how the mesh could be improved.
https://www.dropbox.com/s/619byclo0j...mesh_2_aoa.zip

More arrows mean there are more no of nodes. Fluent / CFD display the velocity field at those points (either in centre or cell faces). If you want to make them smooth then dont copy mesh sizing on far field edges. Instead select them separately and specify uniform spacing.

Also increase the size of edges at these ends some thing like twice or more. In this way you will get uniform mesh at inlet and outlet and hence flow field.


But that all should not affect your solution much if aspect ratio is within range (1000 for single precision and 10,000 for double precision). But you need to check by running both meshes with same conditions.

By default ICEM project faces to surfaces. This is done for blocks at boundaries either internal or outer. For internal boundaries such as wing in this case, when you delete block or change its material, faces are automatically projected to closest surface.

Explicit face to surface association is needed when you want to make wall inside the flow domain.

Could that be the problem that is giving me the random arrow at the wing when I define my inlet and outlets? Or is that a separate issue?

About wing I am not sure what it is showing. Run a sample simulation and see what happens. I think it is not important if wing is defined as static wall.

I did run a sim on both the one you did and mine and yours gave much better results I think.

I am trying to get the script working so I can start making a few of them to test but I just can get it working. What are some common problems people have with scripting? Did you use the replay control when you did the mesh you posted a few posts up?

I think I have a mesh that works okay now https://www.dropbox.com/s/ti1nlnf6js...OA_refined.zip
(fundamentally I mean. i.e. No random elements or weird problems when its imported to ansys)

But even though I have a pretty refined mesh, I am still getting convergence problems with my lift and drag (even at relatively low angles of attack that are below the stall point the values oscillates up and down), which is weird because my residuals are still converging to 10^03 to 10^-4 or better. Note: I know in the pics I took the screenshot a couple of iterations in, but the same thing happened on multiple other sims, it will just keep oscillating like that.

So atm im trying to figure out if it is a problem with my mesh quality thats causing it or if it is becomes of some transient behavior (which would surprise me greatly considering that other people have simulated things like this with RANS before)

place inlet at twice the distance presently it is from leading edge. What are the boundary conditions you are giving it?

Boundary Conds:
Inlet ~76m/s zero gradient air@25C (gives a Reynolds number of 3million)
Side walls are symmetry
top walls are free slip walls
wing is no-slip wall
outlet is average static pressure outlet.

SST with gamma-theta transitional turbulence (high resolution for numerics and advection) (which worked well for my baseline wing)

Is there any easy way to move the inlet without rebuilding the thing from scratch. I cant get the replay control to work properly, it will do some of it then fail or do something random. Its really frustrating having to start from scratch every time I want to use a different wing or change the angle of attack.

Just change geometry and update blocking (less than 100 seconds work ;)). Output mesh. I believe you have yplus below 1 every where.

Flow is transitional at Re = 3 Million ! :rolleyes:

I think I got it to work by doing that way (im not very experienced) but I ended up with a whole pile of blocks around the edge but they didnt seem to be hurting anything so I left them (mesh went crazy if I deleted them)

Yeah, thats why im using the gamma-theta transitional turbulence model. Im hoping that it will play nice and give me what I want haha It was working pretty well with the standard wing. (unfortunately im still fighting with the mesh at the moment)

Will run the sim with the longer domain now to see if that helps.