[AlbertoP]

Hi, thanks Simon.

Actually it is a 2D mesh.
I have just merged quad cells (inner mesh around airfoil) created by ICEM with tri cells (far field) created by ANSYS-mesh.

I checked the tri mesh (created in ANSYS-mesh and imported into ICEM) creating the Fluent mesh file, and it works, so the problem is in the merging operation (I followed your instructions above).

Any idea with 2D mesh please?

many thanks!

[PSYMN]

Have you done the mesh checks in ICEM CFD? Did you see any issues with the single or multiple edge checks?

[cjz]

Hello Simon,
I am attempting to use ICEM CFD to mesh a 3D wind turbine airfoil. My rotor geometry is complete and in ICEM CFD. What I'm looking for is a toehold on how to get started with ICEM CFD in 3D. I'd like to use triangles on airfoil surfaces and stack prism on top for boundary layer cells. From there tets to the extents of the domain with again triangles at the surface. I've spent a few weeks banging away at ICEM with limited success. Long story short, is there a decent tutorial on how to get started on meshing such a geometry?

Any help would be most appreciated.

CJZ

[AlbertoP]

Hi Simon,

yes, I got many many errors of all kinds!

In addition, this is not a good strategy, because it is not a quickly repeatable operation if I need to modify something.

So, I want to change, and stay only on ICEM. So, could you please tell me how to get a tri-mesh around a quad-mesh, matching them? And is possible to have a tri-mesh on more surfaces to better control the growth rate, all matched?

Do you reckon it is a good strategy?

many thanks!

[AlbertoP]

Simon,

got it, no problem, no need a reply...

Thanks again!

[AlbertoP]

Sorry Simon,

I changed idea again.

Is that possible to mesh with blocking (quad) like you did in your video tutorial (airfoil 2d), and then attach around a tri mesh for the farfield? All in ICEM of course.

I created 5 surfaces around the inner surface containing the airfoil (quad mesh) but I can't figure out how to tell ICEM to "start" creating tri mesh from the border nodes of the quad mesh.

Hope I explained well...

Many thanks!

Alberto

[AlbertoP]

...I mean if is possible to avoid to create quad and tri mesh not matching..so then avoiding to editing mesh..create hole..create loop..repair mesh (procedure you told me before).


Many thanks!

Alberto

[PSYMN]

Yes, it is possible... Mesh the hexa (quad) section first. Take care to associate the perimeter edges to curves that bound that section of the model. This will ensure that line elements form.

Then change the Surface meshing type to "Patch Conforming" "Tri". Make sure to turn on the global shell meshing parameters option for "respect line elements", this will make sure that the new mesh uses the line elements around the hexa as a base (instead of the curve sizes set on those curves).

While the blocking based quad mesh is loaded, go into Mesh => Create mesh => Surface Mesh Only...

Change the Input to "From Screen" and select the surfaces around your hex meshed surfaces...

Compute.

This should then mesh just those surrounding surfaces with patch conforming triangles using the line elements around the existing mesh as seeds.

Warning, this assumes the geometry is connected... If you build topology (or color by count), the curves between the surfaces should be red. You will also need to set reasonable sizes for the curves on the outside of the surfaces so they can mesh properly...

[AlbertoP]

Hi Simon,

thanks, got it, and it works. BUT...not well... I mean, the patch conforming is done, but in the part of the curve where the node density is very high, ICEM generates "bad" triangles (long and thin) instead of little uniform ones. In the final mesh there are no errors, so it's good to import into FLUENT, but I reckon it's not good in some areas from a generation point of view.

Any ideas please? Maybe the tool is strong but not enough for a patch conforming on a single curve where the distance between nodes is very different along it?

Another question, about my previous problem. I got a matching between two different mesh (created at different moments) editing them...deleting some cells...creating the loop...remeshing to fill the hole. But as per my previous posts, I got problems importing the mesh into FLUENT. Checking the mesh, I got errors like DUPLICATE ELEMENTS (I fixed them) and MISSING INTERNAL FACES (I fixed them as well). The problem is that some elements edges (the ones for whose I had duplicate and missing internal errors) appear as WALL into FLUENT, and they can not be change into INTERIOR.

Any suggestion also for that, please?

Many thanks for your patience!
Kind regards

[PSYMN]

Some pictures would help...

The long thin triangles problem sounds like your sizes jumped to far and it just connected the nodes on the perimeter of the loop (a fail safe). Are there any nodes on the interior of that surface? You may need to put a smaller size on some of the other sides so it can transition reasonably.

I don't have enough info to guess at your second question.

[AlbertoP]

OK, here's some pictures...

The first three well show you the problem... The fourth one shows you how I would like to get the cells growing (made in another way of course)... whereas the fifth one shows you how I got, I mean with patch dependent I am not able to get the cells growing even if I set curve parameters (like I did in another contest with success).

ps: about my second question...well...I don't know how to better explain... but no matter, I would be happy to solve the first problem.

Many thanks again!
Alberto

http://img828.imageshack.us/i/patchdependent3.png/
http://img204.imageshack.us/i/patchdependent2.png/
http://img807.imageshack.us/i/patchdependent1.png/
http://img141.imageshack.us/i/rightgrowing.png/
http://img269.imageshack.us/i/badgrowing.png/

[PSYMN]

If you want it to be all triangles, you can set the type to "all tri", in the first few pics, the mesher is just trying its best to connect large triangles to small quads... the only way to do it better is to re-mesh the area including a few more cells on either side so the mesher can have some room to adjust sizes...

[AlbertoP]

Hi Simon,

OK, thanks. I figured out that is better to manually do the "matching operations".

About that, just one last question please: since it is a 2D configuration, of course I get single-edges around the perimeters and I "ignore" that.

But I can't understand why I get some single-edges also in a not perimetrical aera. Please see the image to understand where the problem is. (I created a hole around the quad-mesh and then did a re-mesh to get a match between quad-mesh and tri-mesh).

This single-edge problem is only there (and at his opposite corner, below). It is not a real problem to get good results in terms of lift and drag coefficients, but there is an interference in the wake, since FLUENT can not see these edges as interior, but rather as WALL...so the flow impacts on them creating two wakes that are not supposed to be.

Many thanks for your always quick replies!

http://img217.imageshack.us/i/singleedge.png/

[PSYMN]

There must be a topology (geometry) disconnect... You could prevent it with a build topology operation before meshing...

But you can also fix it easily. Go to Edit Mesh => merge Mesh => Merge nodes (with a tolerance). Put in a very small tolerance and select all the elements or the single edge subset, or you could just select the patches where these problems are...

It will merge nodes with their neighbors and the single edges will go away.

[AlbertoP]

OK Simon,
thank you very much for your invaluable support.

Kind regards

Alberto

[AlbertoP]

Hi Simon,

about meshinq with patch conforming between quad and tri mesh... with "respect line elements"... what does it mean if after the mesh computing the inner quad mesh disappear? And only the outer tri mesh (just computed) remains.

Always better doing it manually? Or do know what the problem could be?
Many thanks

Alberto

[PSYMN]

The new mesh shouldn't replace the original mesh, it should merge with it...

Off the top of my head, I am not sure where things went wrong for you.

[Far]

Originally Posted by PSYMN

As a teaser, here are some pics... The total mesh time from geometry to solver was about 15 or 20 minutes.

Simon this post was written in 2010. But I see the technology (multi-zone) used in these pics was made available in ICEM 14.5!!! Did you make this meshing when multi-zone was in testing phase ?

[PSYMN]

Originally Posted by Far

Simon this post was written in 2010. But I see the technology (multi-zone) used in these pics was made available in ICEM 14.5!!! Did you make this meshing when multi-zone was in testing phase ?

I may have posted those shortly before release, but I think it was with version 13 or what ever version we released that year... 14.5 was not the first release to include MultiZone, but it probably did include several man years of enhancements including hooking up Gambit sizing functions and TGrid Tetra. Work on MultiZone continues at a high pace, but work has focused on internal flow and FEA use cases.

[asal]

Hello

I have the problem exactly same as #1 fig 4, over the cut plane. this gonna happen when I want to use Delaunay meshing. there is problem with the Octree!
does anybody known what is the problem as well as the solution?
thanks.