CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   Workbench volume meshing (

skaboy607 January 26, 2011 19:13

Workbench volume meshing

My problem is simple (I hope), A room modelled as a rectangle, a heater modelled as another rectangle within the room and a tube modelled as a radiator also within the room.

What I have done so far...created named selections for the heater, room, and radiator seperately. Two other named selections, the room again to represent the fluid (air) volume and the heater and radiator to represent solids named fluid and solid respectively.

When used in Fluent, it recognises the zones correctly but and doesnt add any default zones (inidicating that I have named everything) but the model does not 'work'. I say it doesnt 'work' because I have used the mesh from tutorial 5 (modelling radiation and natural convection) with the same problem setup and it behaves appropriately. I think there is a problem with the volume meshing/setup maybe I need to subtract one from the other to give the true volume of air (as done in Gambit) but I dont know how to do this.

Thanks in advance for any help you can provide.

jsm January 28, 2011 08:45


Yes. You need to subtract the heater and radiator domains from air domain. For this, in DM, go to the following option

Create --> Boolean --> subtract

Select the target body --> air domain
Select the tool body --> heater and radiator and click generate.

This will subtract the heater and radiator from the air domain. Now you have three domains.

Then select this three bodies and create form new part to get node connectivity in mesh. (This option is available in right click after selecting three bodies)

Hope this will help you

skaboy607 January 28, 2011 14:41

Thanks for the reply, appreciate it. I had previously tried carrying out this method but maybe not quite as you have described, I definately did not create a new part...

I had 4 named selections:

Fluidair-this was a selection of all three but no boolean.

I had also tried the boolean approach with and without an extra body i.e. once using the room and two tool bodies, surely this alters the geometry of the room? and the second time using importing a second body that I could perform the boolean operation with.

When importing into fluent, I get multiple cell zones and interior zones created with all of the above methods?


PSYMN January 29, 2011 21:08

I think JSM is on the right track for fixing your problem, so try it again.

Or, an alternate method would be to create the objects in the room (Heater and radiator), and then create an enclosure for the room (or use the room solid you already have to define the enclosure). When you create the enclosure, it assumes that it will be the fluid flow volume and does the subtraction for you and even gets it ready to pass to the CFD solver in a CHT setup or whatever... Anyway, at the end you will have 3 bodies, not 4.

Then create a multi-body part if you want conformal mesh, or leave it as separate parts if you don't.

Have fun.

skaboy607 January 30, 2011 19:45

Thanks for advice on this however......I am still having no luck with this! Perhaps it is my limited knowledge of the FLUENT/Workbench interface. I didn't think that a selection could be defined as a fluid/solid and also as BC.

I took Jsm's advice and did exacly as described to get node connectivity. Everything was looking good until setting the BC's for the radiator and the heater. It defined them as an interior so no conditions could be set. When changing it to wall, it creates another 'object' called 'orignal name-shadow'? And even then the full list of BC's including the 'convection' term I wanted were not there, only temperature, heat flux and coupled.

If I opted for the 'enclosure' method, could the enclose be defined as wall aswell so that I can specify the wall thermal characteristics.

Any ideas? This is making me tear my hair out.

PSYMN January 30, 2011 19:51

You don't need a boco between boundary conditions... you just need to setup your CHT on those parts. I recommend finding a tutorial. Do you have access to the customer portal?

skaboy607 January 30, 2011 19:55

Er, I'm confused 'boco between boundary conditions', 'cht'? Ya I have access to the customer portal, and I have completed tutorials for Fluent and CFX. I have spent hours/days on them. They are either differences plus there isnt actually a tutorial that takes you through the design stages in workbench and if there is, it isn't similar to mine so doesnt help.

jsm January 31, 2011 05:39


From your reply, I understood that you have good mesh for your geometry and struggling for setting the BC for the model. If I am right, please clarify this for me.

Are you modeling heater and radiator as solid domain or fluid domain? And did you defined the BC for suface zones (like inlet, wall) before going to Fluent?

Give your Boundary conditions in ansys meshing. I think that this is much convenient and good approach for BC settings.

skaboy607 January 31, 2011 06:06

I was satisfied with my mesh when it was seperate parts but when combined, it was an auto mesh and to be honest it looked a bit of mess! But I figured it would suffice to at least get the problem started.

But you are correct, setting the BC's are the main issue...or a combination of both!

In FLUENT, there is only one cell zone that imports which I defined as fluid. In designmodeler, I had 3 names selections: NX_Radiator_Wall, NX_Heater_Wall, and NX_Fluidair (which was the room solid with a boolean subtraction of the heater and radiator). This is what you mean by defining BC's in ansys meshing yea?

When I get to FLUENT, it is where it all goes pete tong. One cell zone: 'part-solid' which I defined as a fluid. And....6 boundary zones identified for some reason: interior-part-solid, nx_radiator_wall, nx_radiator_wall-shadow, nx_fluidair, nx_heater_wall, nx_heater_wall-shadow? What am i doing wrong?

Thanks for all your help.

jsm January 31, 2011 07:50


I think you are not defining the boundary condition for bodies (cell zones in Fluent) in ansys meshing.

For this, select the body filter in ansys meshing and right click on the body (for which you want to define as fluid or solid) to get the named selection option. Then define the name for that zone as you like. Then you can convert the zone type as fluid or solid in Fluent

You can refer the documentation and some tutorials for BC settings.

skaboy607 January 31, 2011 08:19

I'm sure that I have done that. In my previous post, it was the named selection called 'nx_fluidair'?

To get this named selection, I used the body selection tool and selected the room solid after the boolean procedure.


PSYMN January 31, 2011 12:58

Right, but how do you plan to model the solids? Do you want them to be volumes that generate heat and then pass that heat to the fluid? In that case, you need named selections for those bodies also. This would be normal for CHT (conjugate heat transfer).

Or you could go more basic and just create named selections for the boundary faces of the fluid volume that correspond to those bodies (you can suppress those solid bodies in ANSYS Meshing since you don't need them at all for this method), and then you would put a q value or some sort of temperature boco on those interface surfaces. You would have a single volume with bocos and not get any shadow bocos.

You need to pick a method (volume based CHT or face based bocos (boundary conditions)) because it sounds like you are going for both and Fluent doesn't like it.

skaboy607 January 31, 2011 14:02

Yes I would like them to be solid volumes that; the heater with a fixed temperature wall boundary condition, and the radiator and room with wall convection boundary conditions. I thought I had already created named selections for these, on my post, I have listed them: NX_Radiator_Wall, NX_Heater_Wall, and NX_Fluidair. Am i missing something?

Surely you need boundary conditions for CHT too?

PSYMN January 31, 2011 15:26

Great, so just go back to ANSYS meshing and suppress or delete those solid bodies. You don't need them meshed, all you need is their wall on the fluid boundary. Once those bodies are gone, the shadows will go away and you will be back to a very simple problem with straight forward bocos.

skaboy607 January 31, 2011 20:44

OK. Tried this but this doesnt give me the model I require (I don't think). It allows me define the fluid (good) but only one BC. The heater, walls of the room and radiator are all included under one boco?

What I would like is a seperate boundary condition option available for each as they all have different thermal properties.

Also, after running 50 iterations with the wall at a ridiculous temperature, there is no heat transfer occuring? Would I help if I posted my mesh file?


PSYMN February 2, 2011 23:42

Right, so create a named selection for each boco... You could create separate ones for each side of the heater or one named selection for all the heater sides... They just provide names so you can easily apply bocos in Fluent.

See this video I put on Youtube...

skaboy607 February 7, 2011 19:25

Hey, thanks for the video guide, with various changes. I managed to get somewhere towards a working model. I would now like to refine my mesh, it is currently set to the auto settings but I have made it finer. I would however like to create a quad mesh with inflation on the wall surfaces but methods that I have used to do this before dont work on the volume?

Is it possible?


PSYMN February 12, 2011 18:02

Multizone or Cutcel
Are you trying for a Tetra mesh with inflated Quad along the wall?

You model sounds very "boxy" to me, basically some boxes in a rectilinear room. Your best bet would be a Multizone model for pure hex with hexa inflation layers.

Set the method to Multizone, then insert an inflation method and pick the items and floor, etc.

Multizone is basically automated ICEM CFD Hexa, but smart enough to subdivide the volume into sweepable regions all on its own. It then uses OGrid to create the boundary regions.

You may also want to try Cutcel, a Cartesian based mesh method that works well if your solver is Fluent. This is under assembly meshing, a global mesh method (not with the other body mesh methods), but it is pretty easy to setup. Just left click on the mesh branch and then go into the details panel that appears in the bottom left. Turn on Cutcel, and turn on inflation... And compute mesh.

skaboy607 February 12, 2011 18:19

Yea that is exactly what im trying for. It is 'boxy' but there is one complicated part that maybe changes how the meshing should be. I cant attach the geometry/mesh file because it is too large but here is is two link to a picture of it:

I created this part for the third time in design modeler as my IGES import contained 'hard edges' and deleting them deleted faces I wanted in the geometry. I hoped this would solve the problem but it has not.

Also, I can't find the option for Cutcel. Is the details panel the properties panel within workbench? I left click on mesh and within the properties panel, there are no options that can be changed.

Thanks for getting back to me.

skaboy607 February 12, 2011 19:15

Found Cutcel method, it doesnt work on multibody parts apparently.

Multizone method fails too. Unexpected error....something about memory but I watch in task manager and it was nowhere near limit so not sure.


All times are GMT -4. The time now is 20:30.