[siw]

Hi,

In the past when I needed to run a 2D CFX simulation I would made a 3D mesh in CFX-Mesh and use the Extruded Periodic Pair to get a a 2D mesh and this was perfect.

But now I need to run a 2D dynamic mesh simulation in CFX. Which means I unfortunately have to use the dreaded ICEM Tetra/Prism, which ANSYS has forced upon us for the CFX Replay Remeshing - the sooner ANSYS get this CFX remeshing working for ANSYS Meshing Application and/or CFX-Mesh then all the better!

Can ICEM Tetra/Prism (I don't have the Hexa licence) make equivalent meshes? Or can it make a mesh on the face of a 3D domain and extrude it to the opposite face - which is what CFX-Mesh does? If so how would I go about starting?

Hopefully someone has tried this and can let me know (Simon?).

Thanks,

[rikio]

Hi,

I am not clearly understand your thought. But as CFX suggested, you can mesh the 2D model, and then extrude one layer to run it in CFX.

[PSYMN]

Yes, certainly it can be done in ICEM CFD... Or should I say the dreaded ICEM CFD?

If you have 12.0 or sooner, you can use 2D patch conforming (dependent) meshing with your Tetra/Prism key... If you have 11.0 or so, you can still use 2D patch independent surface meshing with your Tetra/Prism key. Either way, you could have tri or quad mesh...

If you want prism, don't for get to go to prism params, Advanced prism Parameters, and turn on BLAYER2D...

If you are going to use the Patch dependent surface meshing, then make sure to setup the curve sizes around the perimeter of the surfaces you want to mesh... Patch dependent uses the perimeter curves to set the sizes, so if you miss that...

Anyway, with either mesher, when you go to compute the surface mesh the default option will be to mesh all geometry... Change that to selected surfaces and select the surfaces you want meshed... You can then run prism on the surface mesh if you have checkboxed prism for the surface and curve parts.

But we could also talk about the root of your problem... What do you mean about wanting replay meshing in Workbench? How about parametric and peristent meshing? Lets talk about that and perhaps you could avoid the dreaded ICEM CFD Tetra/Prism .

[siw]

Hi,

Simon, thanks for the information once again.

I have now made a 2D mesh by creating points and then curves (no surfaces) and have assigned element properties to all the curves (nodes sizes, bunching etc). I have also specified a 1 layer thick quad layer to the walls via the Curve Mesh Setup in my model for edge splitting later (but this created massive quality reduction of the whole mesh and no options for making a good bounday layer mesh). The 2D mesh was made with the Patch Dependent option. Finally, I extruded it along the third-dimension so it's ready for CFX.

I would never have found the Blayer2D option (it's well hidden) which may be better for making the boundary layer elements. I've looked at the v12 Help Manual but it's a bit brief on the details. How do I use it and set up the parameters for my mesh? The compute shell mesh image doesn't show where it's applied. Considering my model has no surfaces, only curves.

So all I need is to be able to get a good quality boundary layer mesh to the specified parameters that I need such as growth rate, number of layers and first layer height.

Now, the replay part is required because (you'll know about this more than me) with CFX v12 there's an ICEM Replay Remeshing feature which allows CFX to simulate models that have moving boundaries and require meshing for the cases were the User does not know the motion before the start of the simulation: i.e. modelling store separation. Therefore, in this case ICEM must be used and the remeshing uses a replay file.

Regards

[PSYMN]

Look under the Mesh tab => Global Mesh parameters => Gobal Prism Parameters. At the bottom of the DEZ is a button that says “Advanced Prism Meshing Parameters”… Push the button and a pop up will give you some options, including “Blayer2D”. Select it, Apply, Dismiss, Apply.

Generate the shell mesh as you normally would. In my case, I usually have a surface, but I think it will work without one also.

Under the mesh tab => Part Mesh setup, you can check box the parts that will have prism applied… Select the right curve parts, and the surface (or at least shell) part.



And here is where we have a bump in the road with 12.0… I think this was fine at 11.0, and has been fixed for 12.1, but the 12.0 GUI did not let you select curve parts for prism, but you could still do it thru the replay script…

Try something like “ic_geo_set_family_params PRISMCURVES no_crv_inf prism 1 emax 5.0 emin 0.0 edev 0.0” where PRISMCURVES is the part name of the curves you want prism to grow on, and 5.0 is the size… I didn’t use width at all. This is for all default settings)

Anyway, I cut and paste that line into the 12.0.1 message window and it worked for me.

Then go to Compute Mesh => Prism Mesh and hit the compute button.


Note: it is not as flexible as regular prism at moving quads and things out of the way, so to get the three layers to form, I had to first merge away an element on the top right side… We are not really focused on this as a go forward solution… All 2D CFD meshing development is being done within the ANSYS Meshing tool, which you should be able to use for your moving mesh application at 13.0

[PSYMN]

One more thought...

You could also use laplace smoothing to reduce the jump in mesh size...

I didn't do anything to freeze the prism layers, but you could freeze by type or part...

See the screen shot.

[siw]

Thanks once again.

Now that CFX can conduct dynamic remeshing studies at v12 I'll be doing lots of this types of simulations (this study is for my MSc research) and moving onto 3D also.

Its very encouraging to hear that Ansys Meshing Application will be taking over ICEMs role for CFX to do this at v13, even though v12 is only a few months old. So from one UK user - role-on v13!!

[siw]

I've switch ON the Blayer2D option in the advanced prism section but there's no check boxes in the Part Mesh Setup for assigning boundary layer.

[PSYMN]

Look up to what I posted on Oct 14th...

But I would say that I rarely use the 2D Prism because the 3D stuff works better...

You could turn your 2D into 3D with a simple extrusion, work that and then just take the front face to the solver...

[siw]

I'm sorry, but I don't really understand what (or how) I need to do to get this 2D mesh, even though I've read through the replys. I have also read your replys to another topic http://www.cfd-online.com/Forums/ans...-question.html and followed that by making a global surface and then extracting the surface of the body that is to move within the fluid domain. But I find that is moves curves from one Part to another Part and cuts off some of the geometry.

However, in either case ICEM now will not even make a surface mesh, it just returns cryptic messages. Yet, I've checked everything and don't see why this is happening. As I'm not changing many settings from their defaults.

PSYMN would you mind casting an expert eye over my model please? If you will can I e-mail them to you as I don't want to post them on a public forum.

Thanks in advance.

[PSYMN]

Yea sure, send it privately... I will take a quick look and keep it between us. Please try to be clear what you need to see.