CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS

ANSYS Meshing + CFX Pre - Mesh Connection/Domain Interface Definition

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By YuguiYo
  • 1 Post By YuguiYo

LinkBack Thread Tools Search this Thread Display Modes
Old   May 20, 2016, 16:43
Default ANSYS Meshing + CFX Pre - Mesh Connection/Domain Interface Definition
New Member
Darryl McClure
Join Date: Dec 2011
Posts: 10
Rep Power: 14
mcclud is on a distinguished road
Hello all,

My workflow thus far has been
  • import .step file into DM
  • delete any extraneous edges, faces, unnecessary details
  • mesh in ANSYS mesher
  • Struggle in CFX-Pre

The problem:

I am currently working with a number of bodies that define a stainless steel structure that encloses a fluid volume (Fluid 1) and the stainless steel structure is then enclosed by another fluid volume (Fluid 2). There will be volumetric heat generation within the stainless steel structure and temperature boundary condition on the outer surface of Fluid 2. Heat transfer across domains is needed.

The SS structure is defined by ~30 bodies so there are numerous faces (~100) that are shared between the solid and fluid 1 and fluid 2.

I have started with meshing each body as its own part as a start and when I move to CFX Pre I am having trouble with the daunting task of manually defining domain interfaces between solid-fluid1 and solid-fluid2. I have noticed that "contact regions" in ANSYS mesher can be grouped by body but when you pass the meshes to CFX-pre the mesh "connectivity" is not grouped in any way as it only recognizes connections where single faces are shared between meshes. I had some hope for the automatic interface generation as I defined each domain but no luck; I just made a larger mess.

Is there any way to pass the contact regions defined in mesher to CFX-Pre? I have searched for ways to define them as named selections but no luck again. My main goal is to simplify the interface definitions when I get into CFX-Pre.

I have also seen a lot of threads where a multibody part is suggested to avoid some difficulties. Is this one of those scenarios? Should I be grouping only the solid bodies into one part then another part for Fluid1 and another for Fluid2?

Thanks in advance for reading and any suggestions you may have.

mcclud is offline   Reply With Quote

Old   June 8, 2016, 05:38
New Member
Hugo Regina
Join Date: Apr 2016
Posts: 23
Rep Power: 10
YuguiYo is on a distinguished road
Hi McClud,

I'm really interested in your post because i'm kind of lost with the connectivity between different bodies and my simulation configuration is close from yours. From now, what I know it's that there is multiple way to connect bodies or made interfaces :

1) By the geometry tool : topology shared for a part that regroup few bodies.
2) By the meshing tool : connexions -> contacts -> contact zone (if shared topology has not been done) or the automatic connection meshing in the mesh editor.
3) In the CFX-Pre with the BC characteristics or with the Simulation -> Interfaces -> Domain interfaces or with the connectivity.

Nevertheless, the thing for which i'm not sure is the influence between these differents tools. Let me explain : if you choose to connect the bodies with the geometry tools, how will that affect the connectivity in the CFX-pre tool ?

In my case, i simulate a heat transfer from an immerged solid in liquid domain. The problem is that I should do something wrong cause CFX don't understand that the heat should diffuse throughout the solid wall untill the fluid domain...

If you got any news for your simulation, let me know. I would be very interested !

If anybody got information for connectivity, help is welcomed

zf007 likes this.
YuguiYo is offline   Reply With Quote

Old   June 8, 2016, 09:02
New Member
Darryl McClure
Join Date: Dec 2011
Posts: 10
Rep Power: 14
mcclud is on a distinguished road
Hi Hugo,

A few questions:
  • How many Parts do you have defined in DM?
  • Are all your bodies in one part?
  • Do you need to have the solid and fluid domain to have conformal meshes?

The following webpage, which is taken from the user manual explains topology within DM and moving to ANSYS mesher:

In my simulation I ended up having multiple multibody parts. Unfortunately, I couldn't have all domains grouped into one multibody part due to hardware limitations while meshing. With multiple parts comes multiple meshes and these meshes need to be connected if they are to interact with each other (heat transfer, fluid flow across). This is done with interfaces which are defined in CFX-Pre.

However, before you define the interfaces in CFX-Pre it is best to identify the interface surface(s) as a named selection in DM or ANSYS Mesher. I did it in the mesher since my meshing involved a decent amount of defeaturing. It is important to note that you need to identify both sides of the interface as its own named selection. For example: Your fluid body should have a named selection on its faces that is something like "FluidSolidInterface-FluidSide" and the solid body should have a named selection like "FluidSolidInterface-SolidSide". Then when you move your mesh over to CFX Pre these named selections will be available to you when defining your interface.

Back to your case; it seems like you have a defined an interface and forgot to enable heat transfer. See the attached image.

Hope this helps
Attached Images
File Type: png Capture.PNG (5.8 KB, 75 views)
mcclud is offline   Reply With Quote

Old   June 8, 2016, 12:01
New Member
Hugo Regina
Join Date: Apr 2016
Posts: 23
Rep Power: 10
YuguiYo is on a distinguished road
Hi McCud, and thks for the answer !

For now I simplify my configuration, that way i can just focus on the heat tranfer.
There is just one solid in water with inlet velocity and a pressure outlet.

The way i'm doing the simulation (i will try to be concise and to the point) :

Geo : I create 2 cube, my solid is in my fluid domain. I'm doing a boolean. Then I don't share the topology because I don't have other solid. (In that CHT CFX tuto they say that the shared topology has to be done only between the solids inside a part). Then i leave.

Mesh : : I just create my mesh with good precision (inflation and sizing are done). Then I leave. (No need for mesh connections)

Setup: I create my domains (fluid then solid). I put the material of each domain. I put my BC for fluid domain (inlet, outlet, wall and symmetry). Then I create a subdomain for the solid, where I set the thermal volume flow (W/m^-3). After that I look at the interfaces solid-fluid (cause I got only solid fluid interfaces), and I check the Heat tranfer button in the additional interface models. Finally i take GGI mesh connection in place of automatic.

Results : The strange thing is that I can see that the heat is outgoing from the solid but not as it should be. It's like the water is no conducting the heat...

I can put picture but I don't know exactly how to do because CFD online ask me to put it on internet before.

Tommorow I will put the CFX outfile if it can help you to see what i mean


YuguiYo is offline   Reply With Quote

Old   June 9, 2016, 08:40
New Member
Hugo Regina
Join Date: Apr 2016
Posts: 23
Rep Power: 10
YuguiYo is on a distinguished road
Hi all,

Ok for me it's good, my simulation finally work (just the simplified one for now).

So in my case the key was to share the topology only between the solids (and no with the fluid) that way there is two mesh for each face at the interface solid-fluid (I still don't understand very well why it is different from solid-solid interface in the process of setting it).

Anyway after that there is nothing to change in the meshing tool.

Then in CFX, I've just put my BC for the fluid domain (velocity & pressure for inlet & outlet, no slip wall, and symmetry). Then I've put my subdomain to create the volumic source (W/m^3), and just check the "heat transfert" button as was mantioned by Sir McCud 2 post before.

I've tried it in transient and steady time for respectively a pulsating volumic source and a continuous source and all is working well ! I can see the conduction inside the solid, and the advection of the heat by the fluid, that's perfect !!

Now i will add the good geometry, a respectful meshing, and a more accurate setup for my simulation.

I'll let you know if there is some people interested about heat transfer from a micro chip in a turbulent flow.

See you all,

Thanks for the help !
zf007 likes this.
YuguiYo is offline   Reply With Quote

Old   February 18, 2020, 12:29
New Member
Join Date: Feb 2013
Posts: 28
Rep Power: 13
techtuner is on a distinguished road
I want to add some information how to create default interfaces in CFX Pre AUTOMATICALLY through Workbench. It's very important feature for huge multibody models.

1. Using ANSYS DesignModeler and/or ANSYS SpaceClaim we have to load and simplify original model. There are we have to create good geometry contacts between pair of bodies.
I highly recommend to set Named Selection for Boundary conditions and for some manual Interfaces in DesignModeler to use it later in CFX Pre, if it requested.
I highly NO recommend to group bodies in parts in DesignModeler. When we are using CFX Pre with multibody geometry and huge mesh (more that 100M), the performance of CFX Pre due to assembling of Bodies into the Parts will be very poor (Pre_ogl process works very slow with this adjustments).
2. We have to load obtained geometry to ANSYS Meshing. There are automatically should be created Connections/Contacts. Usually default connections are low quality and useless. To create them with high quality we have to adjust Tolerance Value in Contact properties. Make sure, that you are using quite small tolerance in comparison with elements size! Later, we have to Repair Overlapping Contact Regions by right click on the Contacts. So, now ANSYS Meshing have to create contacts automatically with high quality.
3. Adjust and create the Mesh in ANSYS Meshing. I highly recommend to use Tetra mesh with ANSYS CFX, or Sweep Mesh, if it possible. By unknown reason ANSYS CFX has some problems in simulations with Hexa Mesh.
If it requested, we may to create Mesh contacts of different meshes: Create -> Mesh contacts in Connection right click submenu.
4. We have to load ready mesh in CFX Pre. We have to setup all domains manually. Later I highly recommend to change properties of Automaic default interface: Case options/General/ to: Interface method - One per domain pair.
5. If it requested set Heat transfer characteristics in options of every automatically created interfaces.

That's all. If all done well, you have to obtain automatic default interfaces for all connected pairs of domains automatically! It's very accelerate performance of simulation of multibody models (with more thar 100 parts).
techtuner is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] No layers in a small gap bobburnquist OpenFOAM Meshing & Mesh Conversion 6 August 26, 2015 09:38
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
Frozen Rotor 1:1 Mesh Connection pharley CFX 5 January 31, 2013 16:15
[ANSYS Meshing] How to refine mesh in ANSYS 14 like CFX MESH Method in ANSYS 12 nsakib520 ANSYS Meshing & Geometry 0 October 5, 2012 01:34

All times are GMT -4. The time now is 22:26.