CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Inputing mesh with inlet outlet,Why? (http://www.cfd-online.com/Forums/cfx/77932-inputing-mesh-inlet-outlet-why.html)

siara817 July 8, 2010 02:32

Inputing mesh with inlet outlet,Why?
 
Hi dear All,
I Generated 3D mesh in ICEM to use it at CFX, but when I import the produced file ( .CFX5), some parts of the geometry like inlet, outlet,... don't exist in the imported file.
Your help is highly appreciated.

mvoss July 9, 2010 04:21

hy,
make sure that you project the faces you want to be named to the corresponding surfaces of your geom. in other words --> premesh first and then unpick everything except your "named part". if you donīt see anything, no projecetion is applied.

hope that helps.

neewbie

siara817 July 9, 2010 06:50

Thanks alot
 
Thanks for your help Neewbie. I attached two picture files, kindly take a look at them.
At first picture, I did as you told and eliminated other parts exept two inlet ( square ones) and outlet ( the circle one), but I can not see when import the mesh to CFX.
At second picture but I changed shape of the inlet and outlet and they came out from the surfaces. However I saw inlets and outlet parts in CFX, I found out that in meshing I have alot of problems that I should go back to ICEM and modify them.
All the best
Siamak

siara817 July 9, 2010 06:53

The picture files
 
2 Attachment(s)
Sorry last time I forgot to attach the files.

mvoss July 9, 2010 07:21

first pic. --> okay you have surfaces in parts which are shown, but you have to tell ICEM that every surface of the created blockmesh within these areas has to be named after the part and i cannot see it on this picture.

scnd. pic.--> seems to me like you didnīt blocked it right. turn on edges in the blocking branch and check if
- every edge(blocking) is corresponding to a line(geom) which means they are showed green --> you can achive that by either associat the to endpoints of the specific line with the two corrspondig verticies or by associating the line with the edge.

how does your blocking look like?

if the blocking is okay, you have to make sure that the surfaces are associated to the faces, just like points--> vercities or lines--> edges

iīm am not sure,but seems to me like that you have inlet/outlet as surfaces within the bigger surfaces of the "room" but in the mesh these parts are more like cubes with 5 faces, like theyīre extruded from the surface but at the same time you dont have your geometry like that.

siara817 July 12, 2010 03:29

Thanks
 
Hi,
I will try to do your instructions and I will try to improve quality of my meshing as you said, and come back to you to ask other questions.
With kind regards
Siamak

siara817 July 12, 2010 07:01

Hi
 
Today, I tried to improve blocking and the problem was solved. I started using CFX and after defining boundry conditions, I sent it to the solver. After running solver, it finished with following error:

ERROR #002100012 has occurred in subroutine cVolSec. |
| Message: |
| A negative ELEMENT volume has been detected. This is a fatal |
| error and execution will be terminated. The location of the first |
| negative volume is reported below. |
| Volume : -0.4005E+01 |
| Location : ( 0.30896E+03, 0.23095E+04, -0.19950E+04)
When I was defining the geometry in ICEM I used negative values for Z axis. the error may come from that cause.

Any kind of your help is highly appreciated.
All the Best

mvoss July 12, 2010 07:46

check for nagative 3x3x3 Determinantes in ICEM

siara817 July 12, 2010 08:40

Negative element problem
 
1 Attachment(s)
In premesh quality, I selected determinent 3x3x3 and highlighted the meshes with low coulumn bar and with negative amounts in horizontal axis.
I wish I did right. I think there is some meshing problems. I tried to improve the quality by O-grid meshing but I could not.
I will try, and inform you.
Thanks a lot for your kindly help
Siamak

mvoss July 13, 2010 06:33

it seems to me like you havenīt attatched the faces properly. The sloped part of the "roof" shows distorted elements. The blocking face is outside of the surface, so the mesh is twisted to match the nearest surface. why arenīt all of your edges green? so they are not projected, right? same for the vercities.not red means not projected to a point.
You just attatched the edges, right?
Where are the negative elements?
not sure: but sometimes it helpes to switch to "project to curves" (right-click above pre-mesh).
just in case: send me your block and tin file, the geom. doesnīt look very complicated, so maybe i can fix this easily.

;)

neewbie

siara817 July 13, 2010 09:56

Thanks CFD master :)
 
Hi Neewbie,
I could not find '' project to curves'', instead it was '' project to edges''. Actually, I tried this one, but the problem remains.
I tried to send you files, but I could not do that here ( says, Invalid file).
Sorry, I am bothering you.
Best regards
Siamak

mvoss July 14, 2010 05:31

did you recieved my message via mail?

siara817 July 15, 2010 06:52

Yes, I received
 
Hi neewbie,
I received and exported the mesh and used in CFX. It worked thank you.
But it needs that I improve even more the mesh quality, since for example the exhaust top of the roof does not have circle shape in CFX.
I will try to improve the mesh and I will ask you some questions:D.
Take care
Siamak

mvoss July 15, 2010 06:58

How does it look like?

neewbie

siara817 July 21, 2010 05:42

problem in output of ICEM
 
Hi Neewbie,
I tried to learn how I can avoid negative elements. Now I have another problem.
I added one box at the middle of the room( it will be as an air cleaner in the room). But at CFX I can not see the box. I tried a lot of time but I could not solve the problem.
Thanks in advance for your kind help
Regards
Siamak

siara817 July 21, 2010 05:49

picture of the box inside the room
 
1 Attachment(s)
I attached the picture shows the box inside the room. I do the sequences as previous time, but when I open the CFX file I can not see the box, also, the part names related to the box no longer exist in the tree menu.
Regards
Siamak

mvoss July 21, 2010 08:14

hi,

you should take a look at the tutorials.
What do you want to calculate? The ventilation and air distribution with and without the cleaner?
Anyways..
You have to cut the air-cleaner out of the surrounding blocking by cutting the existing blocking at the right edges and then put the created block within your geometry of the cleaner in a new part.

if you want to model just smth. like an inlet at the top of the cleaner, you have to create the corresponding faces in your geometry, cut as mentioned and delete the "inner" block of the air-cleaner, and then name everything (e.g. walls_cleaner and inlet_cleaner). you can also create a subdomain and model the air cleaner with an momentum-source as you also want to contribute to the intake of the cleaner.

;)

neewbie

siara817 July 22, 2010 03:31

Thaaaaaaaaaaaanks
 
Hi Neewbie,
I did as you said and the problem was solved. First of all I projected the faces to the surfaces. I could see the air cleaner in CFX but name of the air cleaner parts ( like ac-inlet) were doubled in tree outline. This time I eliminated the block inside the air cleaner and then, just I produced an output file. I opened the file in the CFX and every thing was fine.
It worked out this time.:)
Thanks a lot my friend.:)
Best Regards
Siamak


All times are GMT -4. The time now is 08:48.