How to mesh a packed bed of spheres?

  • 93 Views
  • Last Post 2 weeks ago
  • Topic Is Solved
hamda posted this 12 July 2018

Hi there,

I have got a packed bed of spheres (fuel elements). I am unable to mesh the space between the spheres. I was wondering if I should have a domain  between the spheres? I mean I should create a cube or cylinder around the packed bed of spheres in order to mesh it? 

Also how can I specify zones? I want to specify spheres as solid zones (that are energy sources ) and the space between spheres as fluid zone in which a gas flows.

Many thanks in advance.

Order By: Standard | Newest | Votes
peteroznewman posted this 12 July 2018

First make a rectangular prism at the dimensions that encloses the spheres. Create, Boolean and set it to subtract. The target is the new prism, the tools are the spheres and set Preserve Tool Bodies? to Yes. The new solid can be assigned to be Fluid.

I don't use Freeze hardly ever, so you might have to do Unfreeze since you have been using Freeze, I'm not sure. See if this works.

  • Liked by
  • hamda
hamda posted this 12 July 2018

peteroznewman,

Thanks a lot for your swift response. I will follow your comments and then post the result here.

hamda posted this 12 July 2018

Dear peteroznewman,

Is there any difference to  create a box instead of prism? since creating a box fitted with the packed bed is much easier than a prism. of course I created a rectangular prism but I just ask to learn

hamda posted this 12 July 2018

I followed your comment and now I obtained the following geometry for Fluid zone. Also , when  I created the prism I select "add frozen" since if I didn't select it, the "Boolean" wouldn't work.

 

peteroznewman posted this 12 July 2018

Looks good Hamda!

When I said rectangular prism, I was describing the geometry, not commands in DesignModeler. So Create > Box creates a rectangular prism.

I've never used Create > Prism, but that is not what I meant.

Kind regards,

Peter

 

 

  • Liked by
  • hamda
hamda posted this 12 July 2018

Thanks Peter.

It is so harder than creating a simple box

I have a question related to specify boundary conditions. I specified inlet and outlet. But  I was wondering if it is possible that  all spheres apply the wall boundary conditions with smooth and no-slip surfaces.?  as can be seen in the following picture there are 6 walls that consist of several spheres. But each sphere is a fuel element and generates heat.

Thanks in advance

peteroznewman posted this 12 July 2018

In Fluent, you can specify faces with particular functions such as inlet, outlet, or symmetry.

Faces that are not specified are automatically walls, so you can leave all the spherical faces unspecified and they will be zero slip walls.

The faces of the fluid on the four long sides of the box are going to be symmetry, while the top and bottom face of the box are going to be outlet and inlet.

The spheres can have an internal heat generation.

  • Liked by
  • hamda
hamda posted this 12 July 2018

I worked with fluent before but my geometries were comparatively simple i.e. a cylinder or a rectangular and etc. I used "porous media model" to simulate a packed bed of thousands spheres but now I have to model a slice of that and just a packed bed of few spheres. This time I want to use CFX, since heat generation is a function of time and indeed temperature is a function of time. I heard CFX is more convenient on this issue than Fluent. I worked with CFX too but just for modelling simple problems (assignments ). many thanks Peter for your swift and complete responses.

hamda posted this 13 July 2018

Dear Peter,

Now I want to mesh (Structured hexahedral grids and Unstructured tetrahedral grids) but there is no option to select these kinds of mesh. How can I apply these kinds of mesh in solid and fluid regions?

Thanks

 

 

peteroznewman posted this 13 July 2018

Dear Hamda,

If you RMB on Mesh you can select Generate Mesh and you will get unstructured tetrahedral elements. With Mesh selected, the Details window allows you to set a global element size.

You can apply mesh controls to bodies such as Hex Dominant meshing which will try to use Hex elements but mix in Tets where it must.

For a fully structured mesh of hex elements, the solid bodies must be sliced in DesignModeler into six sided sweepable bodies and put into one multibody part where the bodies can use Shared Topology to have shared nodes on coincident faces.

I see that you could put two planes through the long axis of the box to just mesh 1/4 of the geometry.  Try Unfreeze on all bodies so you can use the Slice with a Plane method I outlines before. 

Save your project, then in Workbench, File > Archive, to create a Workbench Project archive .wbpz file that you can attach to your post, making it available for me and anyone to download and reply with meshing suggestions for you to use. Be sure to say what version of ANSYS you are using. It looks like V14.5  Is there a chance that you can upgrade to the latest version?

Kind regards,

Peter

  • Liked by
  • hamda
hamda posted this 13 July 2018

Dear Peter,

Thanks a lot.

Yes I use V14.5 . Latest version means V19? If I install it , my previous files including geom, case, data will face some problems to be read? I can upgrade it but It takes some time.  I was wondering if  this current version (14.5) is not able to produce the desired meshes?

Thanks

rwoolhou posted this 13 July 2018

You can read the files from R14.5 into R19, but not the other way around. You'll be able to do everything in R14.5 but it's slower and there are many other improvements in R19. 

As you're not familiar with the tools I'd advise going through the tutorials and watching the various YouTube videos too. 

 

  • Liked by
  • hamda
hamda posted this 13 July 2018

Dear Peter,

I followed your comments and created a wbpz file. please find the attached file.

 I just add that Structured hexahedral grids are supposed to be applied is solid region i.e. spheres,and Unstructured tetrahedral grids are supposed to be  applied in fluid region.

Dear rwoolhou

Yeah, I am started watching videos to learn more about Ansys 19.

Attached Files

peteroznewman posted this 13 July 2018

Here is the quarter model I described above, sphere hidden, with a tet mesh without inflation layers.

With just one Named Selection of the faces of the spheres, Automatic Inflation layers can be created.

  • Liked by
  • hamda
hamda posted this 13 July 2018

Dear Peter,

Thanks but I don't know what the holes are  in my geometry? I create a rectangular prism and then subtract it from packed bed of spheres. But these holes were created. are they real holes? since spheres are pure solid and there is no hole on them.  If so, how to fix it?

 

Thanks

 

peteroznewman posted this 13 July 2018

Dear Hamda,

The holes are where the spheres overlap. It's reasonable that there is some finite contact area between spheres since there is the weight load of the spheres and they are not rigid, so it can't be a point contact.

Regards,

Peter

  • Liked by
  • hamda
hamda posted this 13 July 2018

Dear Peter,

Thanks.

Could you explain more what you said

For a fully structured mesh of hex elements, the solid bodies must be sliced in DesignModeler into six sided sweepable bodies and put into one multibody part where the bodies can use Shared Topology to have shared nodes on coincident faces.

What do you mean by stating "six sided sweepable bodies"? As you know my solid region is the packed bed of spheres and how I can slice it into six sided sweepable bodies?  And also could you please explain more this part of your sentence" put into one multibody part where the bodies can use Shared Topology to have shared nodes on coincident faces."

I asked a lot of questions and you answered patiently. I really appreciate it.

peteroznewman posted this 14 July 2018

Dear Hamda,

I made a series of videos that illustrates how to slice up a fluid volume to get a structured mesh. You might learn something from them. You can see six-sided bodies being carved out of the volume.  I started thinking about how to do this for your fluid.  I think the basic unit in your geometry looks like this:

From that block, you can mirror it and recreate the full bed.  That is what I would attempt to split to get a structured mesh, but the tet mesh seemed pretty good.

When a single body is sliced, the mesher will mesh them separately and the nodes at the cut face will not necessarily line up and each coincident face will have its own set of nodes, so the bodies are not connected, they are separate. See this example.

In DesignModeler, if you select those two bodies in the Outline, and right click and select Form New Part, they will be put into a common Part.  Now the mesher knows that they should be connected and it creates one set of nodes on the coincident face and elements from each body are hooked up to common nodes on the face.

Kind regards,

Peter

  • Liked by
  • hamda
hamda posted this 14 July 2018

Dear Peter,

Thank you for providing me with useful information. I really appreciate it. I will watch your videos. The most challenging part of my problem is meshing. I have to mesh my geometry like this (spheres are solid regions and the space between them is fluid region):

I will work on it and then post the result here.

Many thanks

Hamda

peteroznewman posted this 14 July 2018

Dear Hamda,

When automatic inflation was turned on, both the fluid and the solid had mesh inflation layers.

In your example image, I don't see any inflation layer on the fluid mesh, while I do see it on the solid mesh. It is more important that the inflation show up on the fluid side of the mesh.  Also, in your image, I see some fluid between the spheres. What is supporting the spheres if they are not touching?  Is that just a simplifying approximation to make the meshing feasible?

I recommend you begin the fluid simulation with the tetrahedral mesh, because you get that very quickly. You could spend a lot of time trying to get a structured mesh, and what will be the benefit? Better to spend your time figuring out how to setup the physics and how to get the solution to converge.

Kind regards,

Peter

  • Liked by
  • hamda
hamda posted this 5 weeks ago

Dear Peter,

Yes, there isn't any  inflation layer on the fluid mesh. I think since the most important part of that research  was to capture temperature gradient within the spheres (solid region) so the inflation layer was just used on that part. But I concur with you that  we should use the inflation layer on fluid side too.

What is supporting the spheres if they are not touching?  Is that just a simplifying approximation to make the meshing feasible?

Suppose  a cylinder filled with thousands of small spheres and fluid flows through the cylinder. Because of fluid velocity and mass flow rate and operating pressure, these spheres would  have some movements and they are not completely stationary.So it will be some fluid between the spheres.

Yes, You're right, since figuring out how to setup the physics of the problem is more important...Of course I have to return to meshing stage again, since I have  to do mesh independent calculations too. But now it is better to start to set up CFD simulation.  I want to use CFX  but  CFX V19 provides more features than V14.5? Is it more convenient especially to define functions for temperature,..? Is it a big difference between V14.5 and V19?

 Many thanks

Hamda

 

peteroznewman posted this 5 weeks ago

Dear Hamda,

I know Geometry and Meshing, but I've never used CFX.

I recommend you start a new thread in the Fluid Dynamics area to ask CFD questions.

In general, improvements are made for each release and 14.5 to 19.1 represents over 10 releases.

Kind regards,

Peter

  • Liked by
  • hamda
hamda posted this 5 weeks ago

Dear Peter,

I watched some videos and seems  there is some differences between the two versions.

Thank you for providing me  with useful information and videos.

Sincerely,

Hamda

hamda posted this 3 weeks ago

Dear Peter,

Now I am working with CFX and got some error related to boundary condition  when I am running it. Now I have to come back to the first stage to define 4 walls as shown 2 of them in the following picture. I have to specify 4 sides of the geometry as wall and its type in CFX would be symmetry. But as you know spheres are solid and space between them are fluid. I was wondering if I can create 4 plane on each side and then select "name selection" and define it as a wall?So, both spheres and the space between them will be selected and there is no problem to define its type to CFX. Can I do that?

peteroznewman posted this 3 weeks ago

Hello Hamda,

You have a solid body that represents the fluid, which has four faces where you want to apply symmetry. You can certainly put each of those faces and also pick the faces in that same plane that cut through the spheres to be part of the named selection that you will later assign as a symmetry boundary condition.

Regards,
Peter

 

  • Liked by
  • hamda
hamda posted this 3 weeks ago

Dear Peter,

Thanks. Now I did it in my mesh. That's a relief

Sincerely.

Hamda

hamda posted this 2 weeks ago

Dear Peter,

As you know, my geometry consists of two domain; Solid(spheres) and Fluid(the space between spheres). In CFX, when I want to specify boundary conditions, As you see in the  picture 1, I should specify the location.  I want to name the whole my geometry, say "packed bed". So can I do this in meshing stage?  I mean can i edit my mesh and name the whole geometry including solid and fluid regions using "body" (in picture 2)?

Many thanks

Hamda

pic1

 

Pic2

peteroznewman posted this 2 weeks ago

Dear Hamda,

In Meshing, you can make a Named Selection called PackedBed and selects all the solids (filter on Solids) by clicking ctrl-A or RMB Select All.

Regards,
Peter

  • Liked by
  • hamda
hamda posted this 2 weeks ago

 Dear peter,

Thanks a lot.I did that.

Just one question, since I model heat transfer between fluid and solid, so I need to define "solid-fluid interface". Now in meshing stage, can I select the face that is common  between solid and fluid?  as you know I have 2 geometries  and so I was told that I should just one geometry with 2 parts(solid and fluid domains). then  CFX,itself will create interface domain. Could you guide me on this issue?

Many thanks

 

Close