[max.kozak]

Hi all,

I am new to both ANSYS and CFD modeling, and have some questions regarding generating a mesh for my geometry. I need to use ICEM to generate a mesh with hexahedral elements for geometry which I have created using solidworks.

I am attempting to do the block splitting, and am trying to understand exactly what I need to accomplish. Do I want to split the whole block up as much as necessary to delete any empty space where there isn't actually volume? I've attached my geometry from solidworks, which contains multiple cylinders that I have divided into individual parts within ICEM . The fluid enters from one side, fills up the volume, and exits out the other side. Would I need to split up into so many blocks that I can delete as much space as possible around the curvature of the cylinders? I've attached my attempt at the block splitting, and I keep ending up with results that deform the cylinder such that the shape is not really near the original. I know this is probably very trivial for most of you, but I do appreciate any feedback on whether I'm thinking about this correctly and maybe what some next steps are in the process to generate a quality mesh!

[zacko]

Hey I hope I can help in any way. So it looks like your main blocking is good. You split the main block at the height of the lower cylinder as well as the 2 side cylinders. The only thing I would do is to merge the blocks aside from the side cylinders. Because at the left and right where are no cylinders are The blocks can be merged at first and split later. The you can associate all the edges to the curves and when this is done you could start creating new splits how you need or want them.

Sent from my LG-H815 using CFD Online Forum mobile app

[attiquejavaid08]

looking at given figures, i've modeled it keeping a similar look for blocking. check it out. it will give you an idea how to tackle this geometry. good luck.

[max.kozak]

Thanks for the reply! I've attempted generating a mesh with hexahedral elements and have had more success than I was having (I think). However, there are areas in the mesh where there are disruptions and it is not nice and uniform, particularly at the top of the cylinder and the bottom of the two cylinders. I've attached a couple of pictures, and I'm wondering if these discontinuities will significantly affect my results. Sorry for what's probably a simple question, but I'm wondering if there's a way to smooth this out where all of the vertices from the blocking is.

[zacko]

Hey!
One way of refinement or matching the edges is to use "Match edge spacing". You choose a reference edge and a target edge and then the program will match the spacing, so it looks more smooth! https://youtu.be/GZey-MfVaDY. Look the video at 02:50. Hope that helps 👍

Sent from my LG-H815 using CFD Online Forum mobile app

[zacko]

Another thing that you can do, is to merge certain vertices. I attached a screenshot which marks the edges I mean. The edges have a middle vertice which causes a problem for a smooth mesh. So I would recommend to merge these to one of the other vertices.

In some cases, the option to merge vertices causes some problems. Sometimes new edges will be produced (black edges) and than you need to merge their vertices to get the old blocking (really annoyng). Thats what happens to me sometimes. So this could happen but I don't think it will. So test it and let me hear if this helps

[bluebase]

Hi Max,

i strongly suggest you to do the hexa tutorials!
The minimum you should do is the tutorial "Hexa Mesh Generation for a 3D Pipe Junction".
Moreover, have a read of Simon Pereira's ICEM Guide, called Simon's Tips&Tricks. You'll find it in the sticky thread of this subforum...
Especially the last part of this guide is interesting. There're some tipps on blocking structures.

You will learn about so-called o-grids. This is a technique to subdivide a blocking structure. It is the standard approch to fill a circular shape with hexagonals while maintainig good element quality.

You'll also need o-grids for your smaller pipes. Therefore, make yourself familiar with this technique. It's essential and you'll use it often.

I am sure, that you're going to understand it yourself after a quick read!

With regards,
Sebastian

[max.kozak]

Hi there,

I've been working through some tutorials lately and learning a bit more about meshing. I've attempted to fix some of my issues with the mesh that I created by changing the blocking and think that I've made some progress. Now I'm seeing new issues with the mesh that I'm not sure how to solve. The top cylinder has fairly skewed elements that I can't seem to fix. I'm thinking the assymetry could be due to the automatic association of the block vertices to the geometry. There's probably a simple fix but I'm out of ideas on how to correct this right now.

I've attached images of the issues that I'm referring to, as well as my new blocking strategy. I felt that the blocking was strategy was good, but I'm not sure how to fix this issue now. I've also attached a picture of the bottom of the geometry where I was having problems before. This seems to be corrected, but not without the addition of a new issue in the meshing.

As always, I appreciate any feedback!

[attiquejavaid08]

Originally Posted by max.kozak

Hi there,

I've been working through some tutorials lately and learning a bit more about meshing. I've attempted to fix some of my issues with the mesh that I created by changing the blocking and think that I've made some progress. Now I'm seeing new issues with the mesh that I'm not sure how to solve. The top cylinder has fairly skewed elements that I can't seem to fix. I'm thinking the assymetry could be due to the automatic association of the block vertices to the geometry. There's probably a simple fix but I'm out of ideas on how to correct this right now.

I've attached images of the issues that I'm referring to, as well as my new blocking strategy. I felt that the blocking was strategy was good, but I'm not sure how to fix this issue now. I've also attached a picture of the bottom of the geometry where I was having problems before. This seems to be corrected, but not without the addition of a new issue in the meshing.

As always, I appreciate any feedback!

have your performed some mesh refinement on selected outer blocks of o-grid of small pipes? seems so.

if that's not the case, better share your blocking file and geometry here, i'll love to help you out.

regards,
Attique J.

[bluebase]

Hi Max,

regarding your skewed blocks,
you need to align the vertices properly. As i can see in icem-block-splitting-blocking-ogrids.jpg you only cut the pertruded blocks. This is sometimes helpful to keep the block count low. But in this case you see it would be helpful if you extend the cuts (there is a feature doing this), then you will have vertices which you can properly align with "move vertex". Then your mesh can be made straight.

In the third picture, you see some hanging nodes. The reason is, that you somehow changed the level of refinement of the surrounding blocks. Some solver can work with these hanging nodes, some don't. In case you want to reduce the element density in the central block while maintaining the density around, you may use an advanced technique called clamping. In your case you need a reversed clamping technique.
I just had a good read on this topic the other week http://blog.gridpro.com/nesting/
have a look at figure 5a. The other stuff might be too much effort for you case.

In general your present blocking is a big improvement over your first attempts!

with regards,
Sebastian

[max.kozak]

Thank you for your feedback on the issue I was having! I extended the cuts and it fixed the skewed elements. Additionally, I was able to correct the issue with the hanging nodes that I was having. Thank you both, your feedback was very helpful for me!

My next steps are to import the mesh into fluent to begin running simulations and perform a mesh independent test to arrive at the optimal mesh. However, when I do a mesh check in fluent, it says that the mesh check has failed and there cells on a zone that have nodes not connected to all faces. Any ideas on what could be causing this problem?

[bluebase]

Hi Max,

i don't have an idea on the cause yet.

However, there is a Check Mesh feature to search for problems, such as uncovered faces.
Use this tool to find the location of these cells.

Also make sure that every boundary face is associated to a surface (automatically or by hand), and make sure all boundary faces are in parts which receive boundary conditions during the export, such as wall, pressure outlet, or velocity inlet.

With regards,
Sebastian

[max.kozak]

Hello,

I have now been able to successfully import the mesh into fluent without any errors or warnings. I am now attempting to run simulations for my geometry and look at the velocity contours. Whenever I run a simulation, the velocity contour shows the inlet and outlet, and a cluster in between that doesn't represent my geometry. I've attached images of the mesh that I have imported into fluent, along with a velocity contour when I attempt to run a simulation.

The velocity of the fluid entering is 0.001842m/s, which I have selected as the magnitude, normal to the boundary for the inlet. I have also input this velocity in the solution initialization. Just based on your experience, do you have any ideas on what I could be doing wrong to not generate realistic results?

Thanks again for all of your help.

[bluebase]

Hi Max,

it might be helpful to post the last question in the fluent forum now.

Nonetheless, could it be, that you see some kind of iso-surfaces of the velocity (drawn as a mesh instead of surfaces)? Many post procs need surfaces to draw quantities within a volume, such as cut planes, or as in your case iso-surfaces.
Unfortunately, i only have very limited experience with post processing in fluent.

with regards,
Sebastian