Gambit to ICEM, any advices ?
 

Hi guys,

I've been doing CFD for over a year now and I am now familiar with GAMBIT and Fluent. I made complicated calculations in 2D and 3D. My masterpiece was a whole aircraft with a lot of details I even teach the GAMBIT/FLUENT basics in my engineer school.

I recently gained access to ANSYS 13. I am disappointed in the softwares.
I mean, Fluent 13 is absolutely perfect. Everything is clear and the defects of the early versions are now gone. Making videos is now a walk in the park.

But I knew Gambit were not used anymore so I tried to do some meshing using ICEM. I have no negative commentaries about the interface which is pretty nice.
But I just don't understand the philosophy of the software. I miss the volume substraction that worked so nicely in Gambit and I don't understand the point of the "blocking".
I spent a couple hours to mesh a single square box in the middle of a pipe in 3D.
From what I think I've understand the idea of blocking is to separate the volume in different blocks to do some precise and less CPU costy meshes than the results you had with the Gambit's size functions. But given the tutorials I've read it seems that everytime you use a new geometry you have to make the blocks to fit around the geometry. How is that even possible with a whole detailed aircraft ??

The difference between Pre Mesh and Mesh is also pretty dark for me. The tutorials are not as comprehensive and clear as they used to be with Gambit.

So I wonder if any of you switched from Gambit to ICEM and had any advices for me ? It would be a shame to use Ansys 13 only for Fluent and still mesh with the oldish Gambit.



http://d.static.memegenerator.net/ca...1/14081491.jpg

Now it is over year that I have shifted to ICEM CFD.

Previously I used GAMBIT mostly for turbo machinery (2003 to 2012) and did very complex geometries such as highly curved Fan blades with advance sweep and lean, also casing treatments for compressor stall, casing recess for turbine tip flow and separation control concepts in low pressure turbine. As far as the geometry creation is concerned there is no match to GAMBIT (not even design modeler, ICEM and gridgen). But it has some problems like you can only mesh the compressor or turbine the way you have created and if you see that topology is not perfect then you have to modify the geometry which is hell of job (due to circular shape of blades at hub and at casing for blade tip block.

As already said that mesh stick to the geometry topology underlying, so some times in recreating the geometry you may end up to virtual topology which may be not able to make the boolen operations. Another problem was that you may get the distorted goemtry and then you have to redo the complete procedure.

However when I saw my colleagues working with gridgen for meshing the external flows (wing-fin-body configuration) and they were doing great job with high quality mesh and mesh was not dependent upon geometry i.e. you can create connectors irrespective of topology of model (obviously following the general shape of it) and great smoothing function, I have started to work on gridgen but since due to poor handling of geometry with curvature for turbo machinery, I have started to look for other meshing soft wares like Turbogrid, gridpro and ICEM CFD.

We have even tried the evaluation version of Grid pro and liked the way it automatically smooth the mesh and creates the better topology out of no where by using its high quality algorithm. It is to be noted that, it is also top-down mesher like ICEM CFD. We have also recommended our university to buy this software and included the cost into new project with funding from higher education commission for developing wind turbines suited to Pakistani conditions. But unfortunately top management dropped the idea at the last moment as they are already paying for the ANSYS.

I am also working with turbogrid but it is only limited to turbo machinery and (I am stressing here) to the predefined templates with no option of editing. So for routine Turbo machinery simulation, we work with TG and having difficulty (impossible) to mesh the model outside its limited library.

Therefore at last we moved to ICEM CFD for its speed, making the high quality meshes, O-grid blocking and other features which are not available in Gambit and gridgen. Obviously the availability of ANSYS (as compared to Gridpro) is also a major factor. Still we have difficulty to manipulate the geometry, therefore I have to some make operations in Gambit and then export the geometry into ICEM CFD. For example ICEM can not make the spline for more than 100 points and therefore for more points one has the make the two or more curves and then join them. This may sometimes create the distorted curve. Another short coming is the surface to surface trimming. Also it does not have the function of approximated spline fit when imported points have zigzag pattern due to limitation of CAD software. This function to necessary to get the smooth curve with starting and end points fixed.

In starting I did not understand the basic process of blocking and its relation to CAD model. And it is puzzle to divide the large rectangular box to fit the model, which is combination of different shapes. Ironically some times to mesh the very simple model http://www.cfd-online.com/Forums/ans...re-circle.html we have to make the very innovative ideas in ICEM. Another example is the tutorial of the pipe junction , where at first you need to crate one big block and then divide into three parts and two parts horizontally and vertically respectively. 3rd example can be the J-type grid for turbine or compressor blades http://www.cfd-online.com/Forums/ans...ine-blade.html, creating this type of topology is lot easier in gambit (or any other bottom-top approach mesher) and but make this topology in ICEM you really have to think very innovatively and cleverly and may have to combine different blocking options. And I still not able to make this mesh in ICEM. See pictures below. This is also challenge to all ICEM experts.

However when you turn to other side of coin, you shall start to like the ICEM for its features and then you can handle the very complex models in very short time as compared to Gambit. I want to give example of very simple feature of ICEM as compared to Gambit : For example you have very huge model and there are more than 100 hexa volumes and you want to change the mesh density on some edge of any one volume, then due to nature of mapped mesh, you have to specify the same no of nodes on all parallel edges. It is very cumbersome in gambit, while in ICEM you just need to select only one edge and set the no of nodes on that edge and turn on the copy to all parallel edges and rest of work is done by ICEM for you.
http://img11.imageshack.us/img11/3834/jtoplogy.png
http://img51.imageshack.us/img51/2162/jtoplogy2.png

In summary I want to say about situation you are facing as I did:

1. ICEM has steep learning curve and you have to live with it.
2. Gambit is now old technology and I hope the good features (mostly geometry features and few meshing options) may be incorporated in the latest releases of ICEM and ANSYS meshing. Therefore it is good idea to move to new technology as soon as possible. This is in our own benefit.

Premesh is just a outline of final mesh and does not require the resources and when every thing is finalized and quality checks are made and then you create the mesh and export to any CFD software of choice.

Thank you Far for your very comprehensive reply.

I made some other tests on a 2D geometry with a complex circle-like shape. I tried to use blocking but I got 4 blocks with very refined mesh in top/bottom/left/right of my geometry while the 4 other blocks in the corner of the surface were too coarsen. Finally I got some nicer results by not using blocks and use the curve meshes with height and height ratio and Tri Elements on the rest of the goemetry.

Thanks again for your help, I begin to understand the idea of blocking even though the O/Grid never worked for me :)

After a lot of time and trials I get less trouble to export my boundaries but I'm still unsure of the procedure and anxious while exporting in Fluent !

Regards
Charles

can you post a image of that complex shape for which you are not able to make the nice blocking?

check this http://www.cfd-online.com/Forums/ans...type-grid.html you will observe It took me about six months to reach this level. Though geometry is very simple

http://imageshack.us/photo/my-images/21/88051078.jpg/

http://imageshack.us/photo/my-images/21/88051078.jpg/

When I use blocking, is that absolutely necessary to make the blocks fits the geometry with the association. Because in complex 3D geometry like a whole aircraft that would be virtually impossible

What do you mean by "blocks fits the geometry with the association" I think still you are confusing the blocking.

I cannot see the 2nd pic.

http://imageshack.us/photo/my-images/846/87074048.jpg/

These are my first blocks on this model. My previous try is gone and I'm strating over. I meant like in that case, I have a block around my geometry. Is it possible to mesh right away or do I have to use association to associate the vertex to points and edges to curve.
That's not my intention in that particular case, just a general question.

association is necessary. without association meshing shall follow the boundaries of blocks and after association, mesh shall follow the shape of geometry.

So meshing a complicate geometry in 3D can't be done with blocking ?

It is, can be and should be. What do you mean by complex geometry, are you talking about the aircraft with wings and fins? It is very simple to be done in ICEM and in very less time

Far,

Yes, my next project will be the test of this two-seater aircraft that I'm currently building.

http://imageshack.us/photo/my-images/685/buselec.jpg/

Given the fact that I have a very large number of curves and surfaces, what would you recommand as a meshing strategy ?

That airplane is relatively simple compared to jet aircraft or external vehicles that some people do with ICEM CFD hexa...

I think you will eventually agree that ICEM CFD (with its flexibility and Ogrid tool) is a much faster way to handle this than Gambit would have been. Dividing up the volume to get a nice boundary layer would have been very difficult in Gambit.

But you should probably work your way thru the ICEM Hexa tutorials first. I keep meaning to post a wing in a box tutorial... It is easy to do, but as Far says, you need to learn to think about the blocking... Actually, you would have needed to do that for Hexa mesh in Gambit anyway...

In the mean time, you may want to try "Cutcel" meshing in TGrid. It is not quite as pretty as a nice ICEM CFD Hexa mesh, but it is still good enough and the learning curve is easy. Look in ANSYS Meshing for that option.

------------------------------moved here : http://www.cfd-online.com/Forums/ans...-aircraft.html