[Aeronautics El. K.]

Hi all!

Apparently, I need some help again (I'm not very proud about me asking for help all the time, sorry).

I am looking into laminar-turbulent transition in the near-tip region of a wing.
Figures 1,2 and 3 will help you understand my geometry.

I have tried various meshes (fully unstructured domains and blocks, hybrid etc) but I want to try this as well. I have made a structured block around the wing but I left the tip outside. For the surface mesh on the tip, I used the 2D T-Rex and I also created the farfield boundaries and assembled the block (figures 4 and 5). Now the problem is how to populate that block (the unstructured one) with cells.

I tried to just initialise it and it worked. The only problem with this is that I don't get layers around the tip for the boundary layer. Therefore, I tried to use the T-Rex again. I set the tip surfaces as wall with the desired Δs value. However, I cannot find the proper boundary conditions for the rest of the domains. For the domains that are common with the structured block, I tried the "match" boundary condition and the wall as well, and the other domains I set to "match" apart from the farfield on the side. I tried with the push attributes on and off... generally, I think I tried every combination but I couldn't get the block populated.
Maybe I should also mention that I tried the "adjacent grid" boundary condition too, on the domains that are common with the structured block.

What is there that I'm missing? I'd appreciate some help!


Many thanks,

Lefteris

[tcarrigan]

Hello Lefteris,

What version of Pointwise are you using? I ask because you can match viscous structured and unstructured blocks using Pointwise V17.2R1 or later.

Travis

[Aeronautics El. K.]

Hi Travis,

Thanks for taking the time to reply!

I am in fact using the 17.2 version.

I set the structured domains to the "match" boundary condition and the tip of the wing to "wall". Now, irrespectively of whether I have the push attributes enabled or not, or what boundary conditions I apply to the other domains, the block doesn't get populated. I do get 35 layers around the wingtip (0 full) but then (after a while) I get the error message that one or more entities could not be initialized. I've located those problematic cells and they are on the farfield outlet domain. I hope the attached figures will help you form a better view.
I re-initialized the domain and as a matter of fact I deleted it and reassembled it but the result was the same.

Once again, I appreciate it that you deal with this!


Lefteris

[jrhoads]

Hello Lefteris,

This is certainly a frustrating issue I've come across. My first thought is that it might be related to the amount of RAM available. After T-Rex completes, the Iso-Tet generator calls on a significant amount of RAM as seen in the attached image (and even more if you have specified multiple iterations). If your machine runs out of RAM, Pointwise will return the error you indicated and the initialization will fail. As a rule of thumb, you will need about 130 MB of RAM free for every 1 million cells in your final grid. Since your grid looks fairly well resolved, you might want to start there and let us know what you find. It might also be a cell-quality thing, but I thought we could check the RAM first. (For what it's worth, exporting the recombined grid can take a significant amount of RAM too, so make sure you leave yourself a little headroom.)

John

[tcarrigan]

John has a valid point. You'll want to make sure that you have enough memory to initialize the block. Failed initializations can occur if the iso tet mesher can no longer allocate enough RAM to perform the calculation.

However, the problem may be more of a topology issue, particularly near the trailing edge of the wing tip. In order to get the unstructured viscous block to match the structured block, you'll need to get a sense for the growth rate used on the structured "match" domains. I encourage you to watch this video and see how to get a good value for the growth rate, http://youtu.be/UKwz-b3QkF4.

Now, the problem I see is with the trailing edge of the tip. The structured grid around the wing is a c-type topology. However, T-Rex is going to generate more of an o-type topology. Therefore, it will be impossible for the layers on the unstructured side to match the structured domain at the tip and that's why you'll notice it stopping there almost immediately. When it stops this soon, the cell quality in that region is too poor to form a valid tetrahedra and the iso tet mesher fails.

To fix this you'll either need to change the topology of your structured blocks, create a structured domain on the wing tip, or use an unstructured topology for the entire geometry.

[Aeronautics El. K.]

Hi John! Hi Travis!

Thanks for your answers. I apologise I didn't reply sooner.

It hadn't crossed my mind that memory issues could be the reason that block initialization fails. I did check it then. Usually, I have several other applications running apart from Pointwise like Firefox, skype, excel etc... I tried a somehow demanding case and the initialization failed. Then I closed everything but Pointwise and tried again while checking the memory usage all the time. The second try was indeed successful!
Lesson No. x^n learnt. Thank you so much for the tip!

Travis, I didn't put what you said to the test because I changed the whole topology. Insteady of a structured surface mesh, I made an unstructured but very fine one with about 80000 cells on a surface of about 0.056 m^2 and I used T-Rex for everything (surface and block). I have attached a photo if you care to see the result.
By the way, I've watched all your videos on youtube and they are very very very helpful. I've also watched the majority of the CFDMeshing videos (also Chris had suggested one or two of them a few days ago) but I hadn't watched the one you sent me.

Thanks for your help!

Lefteris

[jrhoads]

Hello Lefteris,

Glad to hear you got it sorted out! The mesh looks good too. Just an observation (that may just be due to the cut chosen), it looks like there may be a pretty sharp transition in cell size in the isotropic portion of the grid. If you'd like to slow down that transition, you can increase the Boundary Decay for the block (under Attributes, Algorithm in the Grid, Solve panel) to try and make it a bit more gradual. Since it's away from the body, it may not matter anyway, but I thought I would mention it.

John

[Aeronautics El. K.]

Hi John,

Thanks for checking this out. When I made the cut, I noticed this sharp change in cell size and I didn't like it very much to be honest. The boundary decay is at 0.85 for this mesh. It crossed my mind that I could increase it even more but this would also increase the number of cells in the final mesh and I didn't really want that. My next thought was to change the Aniso-Iso Blend but I wasn't sure this would alleviate this problem and since - as you said - it's not very close to the area of interest, I just left it like this.

Thank you for your comments and help! I appreciate it!

Lefteris