[Hazem24]

Dear Members,

I'd been working on a wind turbine model (3 blades connected at a hub, all surrounded in an inner domain cylinder and an outer domain).

I thought I finally captured the geometry really well (pictures below) with blocks. Turns out there are some negative volume elements (negative determinants) in some areas of the blocks mainly in the connection regions between the inner and outer domain cylinders not at the turbine itself.
I tried PREMESH smoothing which took long hours and actually reduced them but still around 3000 negative determinants remained (out of 24mil) and that was enough to cause "divergence in the AMG solver" while initializing in fluent.

I then tried smoothing and repairing of MESH based on determinant criterion up to 0.2 and 0.0 but it also took almost a day for each and didn't remove any negative volumes.

I wonder if someone has a clue, many thanks in advance! If any other details or snapshot is needed please inform me.

Hazem.
happy massenger.JPG

happy massenger 2.JPG

quality 3x3 determinant (Mess2).jpg

quality angle (Mess2).jpg

[bluebase]

Hi Hazem,

when you have negative elements still present, there is no point to run any solver with that mesh, almost any will fail.
The same is true for smoothing, whether the premesh or mesh smoother.

From the few image, your blocking looks quite nice and advanced. With such complexity of the blocking you might have to tweak some edges and vertices.

In regions where blocks stretch out and follow some curvature in neighbouring blocks the automatly created premesh can squeeze elements into each other till they become negative.

Using the qualitiy histogram is already a good head-start! A small tip is to change the plot boundaries to -1 and 1 and plot an even number of columns, so, you can draw the only the negative elements and find the source of the issue.

The next feature you likely need to resolve those areas is called "scan planes". Its a feature which you find in the context menu of the premesh object ( in the model tree)
It will allow you to draw layer of the premesh in specific directions.

In your case, i would draw a scan plan perpendicular to the "plane" of negative elements, and check which edge is deformed, or which vertex needs to be moved.

At the last step, i would play with "split edge" or "link edge" to prescribe a specifc curvature to edges to overcome the issues in the default premesh computation.

In conclusion, your blocking seems fixable to me. The solution is to find the entities which need individual manipulation.

Best,
Sebastian

[mCiFlDk]

Originally Posted by Hazem24

I tried PREMESH smoothing which took long hours and actually reduced them but still around 3000 negative determinants remained (out of 24mil) and that was enough to cause "divergence in the AMG solver" while initializing in fluent.

I then tried smoothing and repairing of MESH based on determinant criterion up to 0.2 and 0.0 but it also took almost a day for each and didn't remove any negative volumes.

I wonder if someone has a clue, many thanks in advance! If any other details or snapshot is needed please inform me.

Hazem.

Hi Hazem.

I'm not a super expert in ICEM, that's why I can offer another idea: using another ANSYS pre-processor. What I use for complex 3D geometries is Fluent Meshing, it has a very good semi-manual way to fix cells with a wide variety of problems. I frequently obtain many errors in terms of free faces, disjointed cells, negative elements... And thanks to it I'm able to fix it 99% of time.

As a tip I wouldn't recommend to use global smoothers or similar tools, because they distort many cells that don't need to be fixed.

I hope it helped you a bit. Best of luck.

[Hazem24]

Dear Sebastian,

I'm very thankful for your answer !
I've also sent you a private message, could you please see that one too ?

[musa19]

Hi members, I hope you are doing good. I am facing the same problem of negative elements. I tried several ways to fix but unfortunately the elements are not fixing. I request to please help me fix this problem. Thanks in advance. I am hereby attaching some pictures of the mesh. Thank you.

[bluebase]

It seems the respective curve is not well defined.


You need to group all of these curves and associate them to the respective edge.
It seems likely to me, that the unwell defined edge has some sections which you either missed, or weren't obviously selectable. I guess, that's where the premesh's volume mesh detached and tried to get closer to the block's edge, which is straight.

[musa19]

Hi Sebastian, Thank you for your quick reply. I did change the curves but it is messing up with the new curve association. I tried few things but I am not able to overcome this. If you can look into this case and update me about the issue. I will be thankful.
I can share the file with you and please let me know if it is ok for you. Thank you very much.

[bluebase]

Hi Penang,


i am sorry, but i don't work on privately send material here. It contradicts the purpose of this forum in my opinion.


You may share what you can openly.


Best Sebastian




As a side note: I do offer my service as freelancer, in case you need it.

[musa19]

Thank you, Sebastian, I understand your point. I have no issues attaching the file here. I am hereby attaching the link. Can you look into this and update me about the issue. Thank you.

https://drive.google.com/file/d/17iL...ew?usp=sharing

[Hazem24]

I'm working on a multizone mesh for a 3 bladed wind turbine rotor on ICEM CFD, by doing 2D surface blocking then converting the block to 3D and creating an Ogrid.
This essentially requires creating topology first (which was tricky in the beginning to get all the curves red).


The 2D blocking went fine, then on converting to 3D the Ogrid failed!

This is possibly because a surface was meshing on the face of the airfoil at the blade tip (I've included pictures).
I started all over, this time trying to create surface using ICEM Geometry tools (surface from 2-4 curves). which resulted in 2 blue curves at the tip, trying to vary the tolerance results in other blue and yellow curves elsewhere!
I wonder if I can get any clues on how to create this surface and build topology.


The model is found in the following drive link
https://drive.google.com/drive/folde...i9?usp=sharing

Best Regards.