CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Simple Meshing (w/o blocking) (https://www.cfd-online.com/Forums/ansys-meshing/75963-simple-meshing-w-o-blocking.html)

 shohin May 10, 2010 16:50

Simple Meshing (w/o blocking)

Hi all,

i am struggling with some very simple operations in ICEM which are easily done with my "old" software ADINA-F

At the moment i just want to make some very simple model: a 2D parallel plate.
I easily managed to define points (4), curves (4) and a surface (1), and defined the bocos using different parts (3) for FLUENT - so far so good.

Now, i just want to have 10 subdivision on 2 curves (inlet and outlet) and
100 subdivisions on the other 2 curves (walls). Furthermore i want to apply some bias for having a finer mesh near the boundary walls. Nothing really complicated, i thought!

First, I tried using the mesh curve function and second i tried to mesh the surface itself, but which way i have chosen, i never got the desired spacing and number of elements (10*100 = 1000!). :confused:

Can the task be accomplished w/o using this ("strange", sorry) blocking stuff??!

Thanks a lot for your answers and also for all the informations available in this great community!! :)

best
shohin

 Brian_P May 10, 2010 21:10

I am no expert, but I think you are better off 2d blocking. Associate edges to curves then blocking>premesh param> there is a edge function where you can specify # nodes per edge.

Hope this helps

 shohin May 11, 2010 11:37

HI,

Does this mean i have to create a block first and then use the functions
you mentioned?

I will give it a try, although i do not understand why such a simple action is so
complicated...:rolleyes:

 shohin May 22, 2010 06:59

hi,

so i tried the method proposed by Brain_P, but it is still not satisfiying.
I also have no idea which meshing method i should use (ok, no delauney,but..?)

It would be very very kind if someone could give me a small step_by_step "tutorial" of how to generate a simple 2D parallel plate with a structured mesh (finer resolution at the boundaries) (for use in Fluent). Lets say i have the points, lines and defined the bocos already. Do i need a surface?

Alternatively i thought about importing the STL file of the mesh into ICEM, but afterwards i have to delete the mesh for defining the bocos. So i would face the same problem...

thanks a lot for your help...

best
shohin

 vagmakr May 22, 2010 13:46

Hello

First lets make somethink clear.

If you want a structured grid you have to use the blocking technique.

There are some steps

1.Geometry creation or import (so you have curves , vertices , surfaces)

2.2d planar blocking creation

3.At the blocking association menu , associate the blocking edges with the geometry curves (use the edge - curve association button)

4.At the pre-mesh params button in the blocking menu use the edge param button to chose your desired grid resolution

5. Update the mesh and tick the pre - mesh box

That is it nut be aware that you have to chose a proper mesh element size at the global meshing menu and you have to save and output your mesh using the proper output solver.

Hope this helps.:)

 PSYMN May 24, 2010 10:48

Basic steps.

It can also be done with patch dependent meshing (without blocking), but you need to make sure you increase the mapping...

However, I don't think it is any easier to setup mesh sizes on curves than it is on block edges. In fact, block edges are easier because you can copy to parallel.

Also, since the blocking is really structrued mesh, it will produce much better meshes (better mapping interpolation) with less memory, etc. than any other method...

The advantage of blocking over unstructured mapping methods increases with the complexity of the model. Its patch independence also gives it a powerful advantage for poor geometry.

You could use the interactive blocking or the automatic 2D Surface Blocking.

Basic steps for interactive...

1) Create your geometry (4 points, then curves from points, then surface from curves, but actually, you could also create the surface directly from the 4 points) Make sure to put your curves/surface in parts to setup for your Fluent Bocos.

2) Go to the blocking tab, initialize blocking => 2D planar. Don't select anything else, just hit apply. This will create a block that matches your surface.

3) Associate the edges with he curves... For this simple geom, you could use the automatic associate button to take care of this in one click. For more interesting models, you may want to associate interactively.

4) Set up your edge params (this is the same as setting up curve distributions, except more powerful and not constrained to curve segments)

5) Generate premesh, then convert to unstructrued mesh, then output to Fluent.

Basic Steps for automatic method...

1) Setup the geometry and sizes as you had before.

2) Initialize Blocking => 2D Surface Blocking. Hit apply with all defaults. This will mesh a full Car body as easily as it handles your simple square.

3) Turn on the premesh. It may be ready to go or you may want to adjust some edge distributions.

4) When satisfied, convert premesh to unstructured mesh (right click option under premesh), then output to Fluent.

Blocking is not as "Strange" as it may first appear. The separate "blocking" is just a way of separating the mesh topology from the geometry topology, which is a very powerful advantage.

 PSYMN May 24, 2010 10:50

online?

Have you seen the tutorial for the 2D airfoil on www.youtube.com/ansysinc/

Your model would be much much simpler, but this does cover all the steps in a more visual way.

If you have access to the customer portal (or built in tutorials right inside your software) you could check out the 2D pipe junction or the 2D car tutorials.

 shohin May 25, 2010 04:23

Dear PSYMN, dear vagmakr,

thanks a lot for your help...finally, i am able to generate exactly what i want.
And as always, if you know how to do it, everything seems logic and clear, nothing "strange" about!! :)

I used the interactive guide from PSYMN and everything was fine....

Again, thanks to you guys and to this really nice forum...

best
shohin

 All times are GMT -4. The time now is 12:48.