inflation layer issue on Ansys 12.0
I am trying to replicate this tutorial: http://www.youtube.com/watch?v=BhkHa1foWMY applied to my case of a Formula 3 race car front wing I want to mesh.
I am stuck at the bit where the tutorial defines the Inflation Layers. When I select the entire volume (I do not even un-select those surfaces I do not want inflation layers on), then I go to the field "Bondary" to click on "Apply" and, instead of having as result the number of surfaces which the inflation layer is applied on, I just have that field in yellow saying "No selection".
I was wondering if anyone has gone through this issue before.
I do not know if the problem comes from how the geometry has been imported into Ansys, because when in the tutorial the guy does right-click on the geometry, options related to "faces" appear, whereas in my case I don't have them, just options related to volumes. I do not really have a clue.
If anyone would need to have a look at the Ansys file, please let me know and I'll send it.
Thank you very much beforehand.
Face selection vs Solid selection...
For your intial selection problem, just try again... you will get it (I recall having that same issue a few times when I first started). When the details panel pops up, just select the body and then hit apply. Watch that section of the video again...
As for your face selection issue...
Look above the screen... There are 4 little selection icons... The one on the right looks like a green cube... it is for "Select Bodies". The one to the left of that is like a transparent cube with only the top face green... That is for select faces.
David had that select faces ICON on while going thru the demo. I am guessing you had it on "Select Bodies".
So when he blanked that front face of the model, the right click knew to offer him face selection options...
Hopefully, this helps.
Hello Simon, thanks a lot for your so rapid reply.
You seem to know pretty much about meshing features on Ansys 12.
I have solved that problem I mentioned in my last post, however I've found a new one.
I am trying, as said, to replicate that video-tutorial. To do so, I'm chosing the same parameter values (min. size and max size, and inflation layer ones) that person does. I do it like this because I thought that if those values worked pretty well for his geometry, which is much more complex than mine, they should work similarly on mine.
However, after clicking on mesh generation I got this message:
"Error: The mesh generation did not complete because one or more methods could not be inflated".
And no inflation layers are generated.
I reckon explaining the stuff on here is not that easy to understand, so from the following link you can download the file and have a look to my problem if you would want to. There is no rush at all.
I didn't have time to actually run your model today, but I did take a look and have some feedback now... I might run it tonight.
1) You were using the "Pre" inflation with Patch independent... That was what the message was complaining about. Click on Mesh and the Details Panel will include a bunch of stuff. Expand inflation and change "Pre" to "Post" (if you are using Patch Independent). Newer versions make this change for you.
2) Your sizes are not good. They are too coarse to capture the airfoils and too fine to be effiecient with such a large box... This sort of sizing worked in David's online demo because he was interested in all the features roughly equally, but you are much more interested in your wing and its wake than in the far field... I would set the global Max surface and volume sizes both to 0.25 or something like that. I would also set a smaller Min size for the sizing function, down to at most 0.001. You could also set the size on the wing its self (insert sizing, then select the wing surfaces), maybe something like 0.01 would be good.
3) David used Patch Independent on his example because his geometry was not high quality and he really wanted the patch independence... Also, he didn't have huge size transitions to worry about. This is not the case for you. you have relativly simple surfaces that the patch based meshers would do a better job on, and much faster too. I recommend trying the default method with the Pre prism and see what happens... If you have 12.1, it should use the Patch Conforming surface meshing with the Gambit sizing functions and then TGrid Prism and Tetra...
4) Either way, for reasonable results, you will want to refine behind your wing... (to capture the wake). You can size with spheres of influence to set the max size locally, but I would probably try a body of influence (this might be a beta feature in your version, but see if you can find anything about it in the help)...
thanks once more for your so rapid and amazing feedback. All your comments about my interests in this case are just right, that is what I am after.
Also thanks for your recommendations and for you interest in running my case.
I've followed them getting a snapshot at every step I've made and you can download that set of pictures from https://fileexchange.imperial.ac.uk/...0/pictures.zip . Unfortunately it eventually doesn't work either. I explain myself:
- 0.png: shows the very beginning. I select the default option, which assumes patch conforming.
- 1.png: I create the inflation layers, selecting then "Post".
- 2.png: I set the sizes in the sizing field, using your values. I've assumed you said them in meters, so for instance 0.001 would mean 1 mm, which is what I've input.
- 3.png: Then I insert a Patch Conforming Method as shown in this picture.
- 4.png: Then I tried to insert a sizing, but I couldn't see the body sizing option. Do I have to create an external body as shown here http://www.ansys.com/products/images...ures-10-bg.jpg to do so? Actually what is indeed in my version of Ansys (Workbench 12.0) is the sphere sizing one, but it doesn't allow me to modify its center location nor its radius.
- 5.png: Then I click to mesh the geometry and the progress bars stay there for ages. Then I cancel the progress and the error message in picture 6.png is shown.
I don't know if the geometry has been badly imported and that is the very cause of everything, but it looks fine to me.
Thanks a lot once more,
A little bit more.
I think you misunderstood a little bit...
I took a quick crack at it (but forgot to include the refined wake and smaller sizing on the airfoil)...
Do you see how I just used defaults... All I added was the insert inflation layer...
I am out of time for this weekend, but I thought this might help you a little...
thanks for the picture and the feedback. Although to be honest I can't see much from the picture. I'll have a go with what I can distinguish from it.
What I can indeed see is that you didn't create a new inflation layer, but used what the sizing comes along with.
I'm not at any rush, so if you could give me some hints over next week about how to create a body sizing for refining the wake region (do I have to created a separated body and use it as the body sizing reference or something?).
I've managed to replicate what you've done (https://fileexchange.imperial.ac.uk/...EFAULT_try.PNG). However the quality of the mesh is quite poor and that warning about stairstep mesh created at some locations is shown.
I'll try to have go with the body sizing thing and I if I don't get it, excuse me in advance to bother you once more next week :)
Hi again Simon,
one last thing.
I'm trying to define a local sizing based on the wing surfaces (as you suggested), however I'm not able to hide faces to reach those of the wing. See the picture from this link: https://fileexchange.imperial.ac.uk/...hide_faces.PNG
As you can see I've got the mouse selected on the "face" mode and when I right-click on a surface the option "Hide Face(s)" on David's demo doesn't appear in my menu.
What am I doing wrong?
am new person for icem cfd
1.what s meant by inflation in icemcfd
2. hw to improve quality of hexa mesh
1) Inflation is a physics neutral name for boundary layers... It could be a combination of hexa and prism elements that are created by extruding the surface mesh (quads and tris) into the volume (inflating it) with a growth rate that is able to efficiently capture the near wall effects.
CFD users are after boundary layer gradients...
2) That is too vague of a question. Look in the help. Start a new thread if you have a specific question...
Inflation control in Fluent
I had been trying to use the local inflation control in fluent meshing the doamin of a double cone, but every time I am selecting the required face to be inflated the 'details window' is showing "Active: No, Invalid Method". Kindly let me know how should I proceed to solve this problem.
|All times are GMT -4. The time now is 05:45.|