CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] domain interface in ICEM for fluent (

hsn September 17, 2009 21:16

domain interface in ICEM for fluent
Dear friends,
I want to model a simple duct in a solid. water goes through the duct to cool the solid. so here we have tow zones 1-solid 2-fluid.
i want to know how to model the boundary that lay between tow domains for fluent. i tried tow ways and both of them was unsuccessful:
  1. i build a model in DM, I modeled tow domains by freezing the duct and enclosure command {as it is in coiling heat tutorial} then i started an advanced mesh with this model. the output for ansys worked but for fluent, it didn't work. there came two boundary as interface and fluent said one of them do not belongs to a zone. :confused:
  2. i made two IGS models one for duct and 1 for solid. i imported the duct to ICME and then the solid. it asked me if i wanna merge them or replace and i selected to merge. it seemed that i have the solid and the duct with each other. everything went good and fluent read the mesh without problem. but the result showed that fluent had not recognized the duct since no fluid entered the duct.
so help me with this:
  • how can i model the duct and the solid at the same time in ICEM, and how should i prepare it for fluent.
thank you in advance for your time and consideration.

rikio September 17, 2009 22:34

Do you need to get the temperature distribution on solid? If no, you can just set a boundary of wall for the fluid domain. Otherwise, FSI problem should be considered.
For the wall, you can set heat flux, heat transfer coefficient or temperature which was used to get the thermal profile.
BTW, what I mentioned are done within CFX, I am not familiar with Fluent. But I think they are almost the same. :)

hsn September 18, 2009 06:46

thank you,

yes i need the temp distribution on the wall, actually the pressure loss of the fluid and the effect it has is very important for me. that's why I need to model both domains. I have done it in CFX but the results was not satisfying.
still I need help, if any information is needed I will provide.


rikio September 19, 2009 23:43

Could u please describe your model more detail? Including the application background, boundary condition and solution target? Maybe u do not need to get the solid domain involved, if u just want to know the T distribution on the solid-fluid interface.

hsn September 20, 2009 12:11

Dear Rikio,
Actually my primary goal is to find the temp distribution in affect of passing coolant. So I need the solid modeled.
By the way I could get result with CFX so my problem is solved by now. But I’m still avid to know the solution for fluent because I want check them.

Best regards,

PSYMN September 21, 2009 09:45

Material points...
If you are doing two regions for CHT, then you need two material points… Put a solid material point in the one section and a Fluid material point in the other. You really only need one surface between these regions (ideal) but if you have two layers, ICEM CFD will forgive you, but you should check to make sure that you don’t have two separated layers of mesh. The nodes of the interface need to be shared by elements on either side (assuming you want a node for node connection). (You could also mesh the solid region totally separately (with coarser FEA type mesh) and them mesh the CFD portion as a fluid mesh, and then join them in the solver, but I guess that is not your intent.) If you have the conformal fluid and solid tetra meshed, make sure you checkbox the fluid for Prism so that the prism mesh will grow off the interface into the fluid and not into the solid. If you checkbox both materials (or neither) you will get prisms in both directions, which may also be good for CHT since it gives you more resolution in the solid in the direction normal to the wall...

When you output, you will find that you can setup bocos for the solid, fluid and interface region that are appropriate…

wingcollide September 21, 2009 23:26

ICEM-mesh of a simple fluid domain
Hi to everyone.
I am new to CFD and to ICEM. I have to mesh a square prism practically(flow over a flat plate) for now. First I generated an unstructured grid following one of the tutorial steps. I used a global scale factor of 5 and an element size of 64. The maximum element size was set to 2. This generated 16 mil elements. Today I was told first I have to generate a mesh with around 6 mil elements. the problems I ran into are:
-if I create the material point at the end of parts generation( as they suggest in the turorial) some of the parts dissappear.
-my mesh doesn't generate everytime( it does- but is just a tetrahedra and it says my mesh has holes in it)and some of my parts dissappear after the mesh creation
-today I generated a mesh using a global scale factor of 2.5 and an element global size of 34 -this resulted in 2 mil elements.
Do you have any suggestion on how to pre-estimate my number of elements-or what my mesh inputs should be, given the number of elements I have to get and my domain size???
another problem is I don't know how to make the mesh more dense in the boundary layer( can I edit the mesh after computing it or are there options to set it up before computing the mesh??)
thanks in advance for any reply

PSYMN September 22, 2009 10:10

For Camelia (who jumped on the end of this post)
Hey Camelia,

1)I am not clear on your mesh sizes… What do you mean an element size of 64 and a maximum element size of 2? Do you mean you set 64 as the global maximum and 2 as the maximum on entities or parts? I hope so. Otherwise the smaller global maximum would dominate.

2)If creating a material point causes parts to disappear, something is very wrong. I have used ICEM CFD for almost a decade and never seen that. Do you mean they turn off or they are actually lost from the tetin file?

3)If parts are disappearing as you said above, then that could cause trouble. If it is just giving you tetras, did you then try and run prism separately? Before Prism can be successful, you may need to check your tetra mesh for errors, etc. I usually run Tetra and Prism as separate steps with a check mesh and possibly some repair between.

a.When you say some of your parts disappear during mesh generation, I assume you mean there is no surface mesh, not that the actual geometry has disappeared. This is probably due to leakage. With the Octree mesher, if the same volume appears on either side of a surface, it assumes the surface is a mistake. It only extracts surface shells from exterior surfaces or surfaces that are between different material points. One way around this is to mark the parts as baffles; baffles can have the same material on both sides and will still produce shells. Then you can close the holes with the mesh editing tools, etc. Alternatively, you could create material points (solid or dead) in each part so that if there is leakage, you will be alerted and can trace the leakage path to find the hole.

4)Look for posts on CFD online regarding the OCTREE powers of 2… I have already written about this several times to explain that your 34 may have been rounded down depending on your smallest size, etc. It is tough to estimate the total size if you do not have a uniform distribution. The size changes depending on how much surface area you have related to the volume area and the difference in size between them, etc. If you did have a uniform distribution, you could divide the volume into equal sized cubes and then multiply by 12 tetras per cube… ie. If your model was a Cube of side 64 and you had uniform size 2 mesh, you could say that you would have 32 cubes on a side, and there fore should expect about (32^3)*12 Tetra elements. If you had a Sphere, then you could calculate the rough number of size 2 cubes using the equations for the volume of the Sphere… Most CAD programs have a way to calculate volume of any shape. Obviously, if you are using a curvature and proximity based sizing function, there are just too many unknowns to calculate well.

a.Knowing what sizes to set for a particular model will come with experience, but you can ratchet it using the scale factor. I usually start with a scale factor of 1 and setup my sizes with powers of 2. (1/4, 1/2, 1, 2, 4, 8, 16, 32, 64, etc.) Then if I was told I needed it to be 20 percent coarser, I would adjust my scale factor to 1.2 (or 1.11 actually since this is a linear scaling and the number of elements changes with the volume).

5)Yes, you can make your mesh more dense near the wall… If you mean tetra mesh, you can set the width parameter on any entity or Part to increase the number of layers before the mesh starts to transition to the volume size. You could also reduce the ratio or add a density box. Of course, the best way is with Prism. Look in my outgoing folder for a ppt of tips and tricks.

wingcollide September 22, 2009 21:21

Thank you a lot Simon. Today I was able to create meshes and I didn't have the geometry dissappearing as yesterday. Also, thanks to your reply towards the end of the day I managed to make the mesh more dense( I used the density box. I will try some of the other methods u mentioned as well). I still have to play with the scale factor and with the global element size in order to get my 6 mil nodes.
I wanted also to know if for CFX is better with a prism mesh then with a tetrahedra one, or in general the adavantages of one over the other.
Thanks again,

PSYMN October 12, 2009 14:12

Generally, for CFD, a Tetra/Prism mesh is better than just using Tetras for capturing wall physics. Prism mesh is important to get more nodes normal to the wall without increasing the number of nodes along the wall. This gives more calculation points necessary for efficiently calculating the viscous effects near the wall (boundary layer velocity profile).

wingcollide October 13, 2009 11:18

Thanks for the reply.I discovered since my second question how prism is better than tetra.I also noticed that tetra may look nice( uniform on the surface) but in the inside the volumes are increasing in size towards the center so I decided to do my entire mesh with prism layers(I can control the number of layers and it gives uniform voulmes even in the inside)The problem I have now is that it doesn't create the last layer- the one attached to the top surface- it leaves it with tetras and I am afraid this will create errors in my simulation. I don't know if it is because I only specified the top surface in the global mesh set up and didn't check it in the parts as a prism part Or if because I didn't put enough layers so the last one has the top on the surface. Let me know if you know why this might happen to my mesh.
Thanks once again for your answer.

PSYMN October 13, 2009 17:16

Prism and Tetra are supposed to work together...
Unless you are talking about sweeping prism from one side to the other (swept mesh), you should expect some tetras in the middle. Actually, you usually expect more tetras than prisms in a tetra/prism model...

For instance, if you are putting prism on the walls of a cylinder, there is no way for the prisms to connect across the middle (unless you have some sort of singularity), the core is typically filled with tetras.

The prisms are just for the boundary layers near the wall (typically less than 1/3 the diameter of the pipe.)

wingcollide October 15, 2009 10:19

Thanks for your answer.My domain is a rectangular cuboid and I believe it is possible to get rid of all the tetras. If by sweeping prism from one side to the other you mean building layers of prisms from the surface to the top of the domain then that is what I really need. I got almost the entire mesh with prism layers except the top one wich is still tetras and I am trying to make it a prism one as well.Please let me know if I can make my mesh entirely with prisms and if there is an option to sweep prisms from the surface to the top.

PSYMN October 16, 2009 09:25

Extrude or Sweep...
You could extrude the surface mesh from one side to the other... You can type in equations to have it grow a certain way, etc.

You could also use ICEM CFD hexa to create a swept block (easiest method if you have the tool)

If you really are close to the other side anyway, you could mesh edit your way out of the problem. Delete the tetras and other shell elements trapped at the end (box select with shells and Tetras displayed). Then run the Mesh checks... It will complain that you have "uncovered faces". Fix the problem by selecting the name of the top part. This will create a layer of shell elements in that TOP part to cover the exposed Prism elements. Then turn on just that part and use the option to project nodes to surface. Since there are no other parts, you will see the nodes jump the rest of the way to the surface stretching the prisms along with them... You may have some other manual mesh editing to do to sort out curve projections, etc.


wingcollide October 28, 2009 19:31

Modify element's angles
I have used your advice and I managed to do the prism mesh(by projecting the nodes). Unfortunately my professor told me he wants an unstructured mesh in all 3 directions and he wants me to test 2 types of tetras: one with angles around 60 degr. and one with angles( by angles I mean the top vertex angles of the tetra) greater than 90 degr so I can have a sense of the error the second type is introducing. I told him I didn't see any options in ICEM about the element's angle and he argued that this program "can do anything (except a spaghetti dinner)" so I went back and tried to make the two types of mesh. I really can not see something that specifies the element's angle( -I noticed that for wider angles the quality is smaller and Ansys Icem is trying to make the quality better. I saw that one can check for the tetra special which is related to the element angle, and also I saw that one can specify the height of the first element layer in the part set-up part-but I am not sure if this or the surface settings will be considered in the mesh generation).
Please let me know your opinion.
Thanks again,

PSYMN November 2, 2009 20:06

Mesh methods.
4 Attachment(s)
Hmm, the angles of a triangle add up to 180, so if one angle is greater than 90, then others must be less.

If he really just wants to test poor quality mesh, then perhaps we could stretch your model (say by 2 in the x dir), then mesh it, and then squish it back down again.

But probably, he is wanting you to compare "Octree" mesh which produces regular 90 degree tetra elements, and Delauney or advancing front mesh, which is closer to equilateral.

You can do this simply by changing the method.

Start with Octree Tetra, save that one for the one run. Then delete the volume mesh (keep the surface mesh and/or prisms) and remesh with Delaunay or advancing front from the existing mesh.

It will look something like these pics. The TGLib with AFT is a 12.1 option, but the rest are available in older versions of ICEM CFD. The last pic is supposed to be animated, but that doesn't work here.


wingcollide November 3, 2009 10:26

Thank you Simon.I will try what you suggested.

wingcollide November 22, 2009 17:09

Surface orientation
I was trying to get less elements in the x direction and keep the same number of elements in the y direction and I scaled my mesh 3 times in the x direction. then I deleted the mesh elements outside of my geometry and projected the nodes on the uncovered faces( as you told me to do with the prism elements near the top surface).Unfortunately after that my mesh check is showing me surface orientation problems( 14 -16) and I really don't know what to do with them.
Let me know what do you think about this problem.

PSYMN November 23, 2009 16:07

Squish and stretch...
1 Attachment(s)
Hey Camilia,

You may have got yourself into trouble when projecting to the geometry... This is not how I suggested doing the squish and stretch technique.

I recommend scaling your geometry by 1/3rd in the squish direction. Then mesh it uniformly so everything is properly projected already. Then Stretch it out again (scale up by 3 in that same direction).

This avoids all the mis-projection issues which must have inverted some of your elements.

I am attaching a screen shot from my tips and tricks 2008 ppt.

Best regards,


wingcollide November 24, 2009 15:26

Mesh stretch-squish
Hi Simon!
Thanks once again. I solved the problems by doing exactly what you told me to do.It was so easy.I don't understand why I complicated my self in the first place.

All times are GMT -4. The time now is 11:27.