[student123a]

Hi,
im new to using ICEM from ansys, and i have been running into quiet a few problems when trying to mesh an airfoil in the program. Ive drawn up the airfoil and have created a boundary around it, but I dont know how to mesh it properly. When i try to mesh the boundary, I cant define the cell size and i cant get ICEM to recognise the airfoil itself (the mesh goes straight though it)

Can anyone help me?

Many Thanks

[PSYMN]

I assume you are using Hexa... Blocking requires a series of splitting, associating, removing blocks, assigning edge params (mesh sizes), etc.

Once you get going, it is easy, but CFD-Online can't get you going from nothing. Try some tutorials... they are built right into the help in version 11.0 or on line for version 12. There are some nice 2D Hexa tutorials you can start with before moving into 3D that will cover all these basic steps and make the airfoil seem pretty easy.

You could also look on line for demos... www.ansys.com/demoroom

[apantune]

Originally Posted by student123a

Hi,
im new to using ICEM from ansys, and i have been running into quiet a few problems when trying to mesh an airfoil in the program. Ive drawn up the airfoil and have created a boundary around it, but I dont know how to mesh it properly. When i try to mesh the boundary, I cant define the cell size and i cant get ICEM to recognise the airfoil itself (the mesh goes straight though it)

Can anyone help me?

Many Thanks

Hi,
you can do this in three steps.

Step One:
a) generate a background mesh ( containing the farfield boundary and your profile boundary)

b) For your profile use the Mesh -> Curve Mesh Setup to define the elements size along it.

c) Generate the mesh using the Compute Mesh -> Patch Independent ( you need to have a surface defining your computational domain)

As you mentionned it will generate the mesh all over the domain....save the project...

Step Two

a) import your profile curves
b) generate a quad mesh using the Blocking menu (Pre-Mesh -> Convert to Unstructured Mesh).
c) Save the project

Step Three
a) Open the project one.
b) Open the project two
c) You will see a overlaped mesh....dissable the quad elements (Mesh -> quad elements)....now delete some tri elements...make a hole around your quad mesh....
d) Use the Edit Mesh -> Create Element -> Tri and link the tri mesh region with the quad mesh region ( you just need to create two elements )
e) Use the Edit Mesh -> Repair Mesh -> Mesh from Edges...select on edge that belong to the boundary where you intend to generate the connecting mesh...and type L on your keyboard....and apply....
f) You should have a nice profile mesh with a prism cap.
g) check the normals ( Edit Mesh -> Re-Orient Mesh -> Re-orient Consistent)...
h) save the project...

In general terms these are the main steps.....

Regards,
Alex

[teguhtf]

Hi Guys!!!
What is difference of Meshing & Making Geometry In ICEM CFD & ANSYS WorkBench??
What is the criteria of our success meshing in both of them??
Thank You!!!
teguhtf

[PSYMN]

The geometry tools for each are completely different.

ICEM CFD is a surface based modeler built on DDN technology (ICEM SURF). Everything is built bottom up, which provides a lot of flexibilty, but makes it difficult to do things like adding or removing fillets. The biggest advantage is that it accepts very poor models. It even accepts combinations of Faceted data, b-spline data, and mesh.

Workbench Geometry is done in DesignModeler. This is a solids based tool built on the Parasolid kernel. Its advantage is that it is a modern tool which can easily do solid operations like Booleans, adding or removing features, parametric changes, etc. Its only problem is that you need relatively decent geometry (or you must fix your geometry to make it decent, sew it into a solid). ALso, 12.0 does not yet support faceted data, etc.

The meshing between ICEM CFD and ANSYS Meshing (Workbench) overlaps quite a lot... The same libraries and execuables are used and the synergy is only increasing with each release. However, ANSYS meshing lacks the controls and interactive tools that ICEM CFD has. In other words, if you ran the ICEM CFD meshing in an automtatic mode with a subset of the controls, you would get exactly the same mesh out of ANSYS Meshing... But ICEM CFD offers the ability to take it another step with more controls, mesh editing, sloppier data, etc. On the other hand, ANSYS meshing makes up for this by its ability to combine methods not even available in ICEM CFD. For instance, the combination of surface meshing with the Workbench sizing function is a good reason to do that sort of thing in Woorkbench rather than ICEM CFD, particularly to get the nice smoothly transitioning surface meshes that CFD users often want.

[teguhtf]

In GAMBIT our good meshing is <0.85. I've tried to convert my GAMBIT mesh to ICEM CFD. My value of meshing is about 0-0.65. but when i convert to ICEM CFD the value about 0.3-1. What is the value of meshing both of ICEM CFD & Ansys??
Thank you for your explanation!!
teguhtf

[PSYMN]

The simple answer is that the range is just inverted... In Gambit, quality of 0 is good, 1 is bad. In ICEM CFD, 1 is good, 0 is bad.

However, the metrics are each calcualted a little bit differently so in your case, 0.65 in Gambit is approximately 0.3 in ICEM CFD.

These are crossing over. For instance, ICEM CFD 12.0 now includes a TGRID SKEW metric that will give the exact same numbers as Gambit... Also, the next version of TGrid includes an "ICEM CFD Quality" metric that will give the same result as ICEM CFD (very popular for prism).

Their are lots of metrics supported by ICEM CFD because the needs change from from solver to solver... For instance, some solvers are very concerned with skew but not at all with angle. Others are more concerned about aspect ratio or volume change... Check with your solvers doc to find the specific requirements. And then you can usually cut that in half since most solvers are being conservative so they can blame problems on the mesher.

Assuming you are using Fluent... you want ICEM CFD quality greater than 0.1 or 0.3... Angle > 9 or 18 degrees. ICEM CFD is particularly critical of prism mesh, so anything over 0.01 is usually good for Fluent. And you can always use the TGrid Skew metric... Try to get under 0.9 or 0.95.

[priya_c45]

hi,
i am a final year graduate student in aeronautics.i wanted to simulate the von karman street in ICEM CFX. i am new to ICEM. All i know is how to make points and lines .I have doen fluent and gambit .is it possible to simulate this in FLUENT?can i get some help with this please

[PSYMN]

Yes, of course it is possible, but ICEM CFD is a mesh generator not a simulator. (the CFD part of the name is unfortunate).

I assume you plan to use 2D? Basically a circle in a box far field?

You can create points (XYZ) for the corners of the box and points for the center and 2 surface points of the circle.

Then draw lines to connect the corners of the box and use circle from 3 points to create the circle.

Then create a surface (in part FLUID) from 2 to 4 curves and select just the curves of the box.

Then Build topology, the circle will be cut out of the surface you just created.

Then delete the circle surface.

Put the inletlet, outlet, and circle into their own parts.

Set sizes using params by parts. Set a width and initial height and ratio on the circle part as this will give you boundary layers.

Mesh using patch dependent all tri

Output to Fluent...

If you couldn't follow this, try some tutorials first.

For help with the fluent setup, I think there is a tutorial for that also, but you could also ask on the Fluent forum.

[priya_c45]

i tried doing the same thing in gambit and fluent...i made the thing as u said..but i am not able to simulate it as a flow....and how to i see the animation part in fluent?

[teguhtf]

Originally Posted by priya_c45

i tried doing the same thing in gambit and fluent...i made the thing as u said..but i am not able to simulate it as a flow....and how to i see the animation part in fluent?

Hy Priya,
for simulating by using point, you can use this thesis.. this works on GAMBIT http://web.missouri.edu/~solbrekkeng...is_logsdon.pdf
hope it helps
teguhtf

[priya_c45]

i have done airfoil simulations before... but what names do i give to the zones in the von karman simulation?
and the details to be fed in fluent?

[PSYMN]

The names don't matter. You can call the sphere "SPHERE", but it will just be a wall. You should have an inlet and an outlet... I am sure there is a tutorial out there on all the transient settings you would need.

[priya_c45]

inlet as- velocity inlet
outlet as -pressure outlet
are these ok?
and what abt the settings in fluent, as in material type viscosity and all.
should it be oil or water?