Meshing problem with ICEM
3 Attachment(s)
Hi to everybody,
I am a newbie with meshing and/but try to mesh a cylindrical furnace with a concentric cylindrical heating element. The air inside the furnace is connected to the surrounding area via two cylindrical drill holes (air inlet, air outlet). First of all I only try to mesh the air (neiter insulation around the air, nor heating element) with a volume mesh. Is it possible to add surface meshes for contact areas air/insulation and air/heating element??? I've tried to work with blocking and o-grids but awfully failed at the positions where the drill holes are connected to the air volume, :(:(:( although I spent really much time. How can I adjust the meshes of the air inlet and outlet and the air volume mesh??? Please help me! Since the heating element does not belong to that mesh I need to delete the central block. Aylalisa |
Associate face to surface (in the area of destroyed elements). If it doesn't work, use interpolate.
You've to provide your .tin and .blk files if you don't get rid of the bad elements Quote:
|
2 Attachment(s)
Hi energy,
thanks too much for your support :). 'Face to Surface > Part' and 'Face to Surface > Interpolate' helped me to get the attached models. I've tried different proceedings: Strömungsraum_6: bottom-up I've generated three blocks and then directly used O-Grid. With help of 'Face to Surface' I've reached that result but still receive quite a couple of bad cells. Strömungsraum_8: top-down I've decomposed one big block in several small blocks, deleted some and finally merged the small ones together again. 'Face to Surface' has provided me that result. Could you tell me how I can get rid off the ugly cells in Strömungsraum_6? What strategy is in that case the best? My final goal is to simulate the heating element (solid) and the air (fluid) that is heated up by convection and radiation. So I will end up with two meshes. Do you know if I have to build two individual meshes or is it necessary to built both in the same model, if that is possible at all. Aylalisa |
I'll check it tomorrow. I'm out of office today.
Regards, Christoph |
With your project number 6, the main problem is the edge of the O-grid of the cylindrical drill holes. They are associated to a surface (colored in black) but there are inside the fluid (they should be colored in blue).
I think you didn't associate the face to surface in the good way. So use the tool "Blocking -> Blocking Associations -> Disassociate from Geometry -> Edges" and select those edges. They will turn in blue which will fix your issue ;) |
2 Attachment(s)
Hi Alexandre,
thank u for your help!!! That worked :eek:, but still there are (only) a few skewed cells :mad: at the intersection where the drill hole meets the main pipe. Why did that deassociate thing exactly work? Do you know repair for the remaining skewed cells? Refining the mesh does not really remove that skewed cells but unnecessarily increase the number of cells I think :confused:... Plenty of regards :) Lisa |
There is problem in blocking. Did you merge the vertices at some stage? Check through scan plane in the two pipes
|
Hello Far,
thanks a lot for your reply!!! I've not merged vertices but I've cut one big block in many small ones, deleted some and merged them again before I've used o-grid. Is there maybe a possiblity to get rid of the bad elements without starting the whole procedure from the beginning? What kind of proceeding is in that case the best one: Start with one big block, cut in small ones, delete and merge to adjust the geometry, or create three blocks: one for the main air volume and two additional small ones for inlet and outlet air pipes??? In each case I end up with a couple of bad cells, even if I don't merge vertices on the way?! Do I make a principal mistake or could I improve the mesh quality by local adjustments? Viele Grüße Lisa |
1 Attachment(s)
Angle > 34 deg
Quality > 0.5 Steps 1. One bigger block and o-grid. Delete inner block and associate edges to curves. Snap vertices. 2. Split at appropriate places (four along bigger pipe and two on two sides of smaller pipes). 3. Draw two curves through centre points in smaller pipes (see in attach files) and use extrude along curve option to extend blocking in smaller pipes and associate curves at the end of pipes and at intersection with larger pipe. 4. Make ogrid for smaller pipes. Select two blocks (one for smaller pipe and one in the larger pipe touching heating pipe and select two end faces) 5. Assign sizes on surfaces through part mesh setup (maximum size 3) and click on update all (blocking>edge mesh parameters> update all). And if necessary set the edge mesh parameters for the o-gird edges in the smaller pipes genießen :D http://imageshack.us/a/img217/8973/pipe2002.jpg http://imageshack.us/a/img213/1787/pipe2004.jpg http://imageshack.us/a/img826/9918/pipe2003.jpg |
Quote:
1. Your both approaches are producing the problem elements? 2. Do you need solid blocks? |
1 Attachment(s)
Hello everybody.
aylalisa. If it's geometry for CFD calculation I will do enouther blocks for this geometry. 1. You need boundary blocks. In attach file you can fine my solution. The first errors was in black edges. The second in blocks. :) |
1 Attachment(s)
Quote:
Also check this blocking ... |
Wow!!!
A very big thank you for all your approaches!!!! :)
I will figure out now to see if I can follow! I am happy :):):)! Lisa |
error message: extrusion of faces failed
2 Attachment(s)
Quote:
May I ask you for detailed hints, especially according to the first three steps? 1. O-Grid ( ) without selection of top and bottom faces ( ) with selection of top and bottom faces I've decided for the latter option. Association: outer edges of remaining blocks will be associated to outer circle inner edges of remaining blocks will be associated to inner circle (center drill hole) 2. split at appropriate places why 'four along bigger pipe'? After 'snap vertices' it seems that there is only need for two splits along bigger pipe? --> screenshot I understand 'two on two sides of smaller pipes'. 3. extrusions for smaller pipes no problem with creation of two points, no problem with creation of two curves, BUT: I always receive an error message if I try the 'extrusion of faces' --> screenshot This also happend all the time during earlier attempts. Why? Finally I gave up to try using the extrusion command. I use ICEM v14 on Windows 7 :mad: I thought I make some mistake but according to your description the usage of this command seems to be all right in this context. Can anybody help??? Lisa |
1. Are you using extrude along curve option?
2. Are you selecting the correct face? Quote:
Quote:
|
Now it works!
1 Attachment(s)
I've always tried the steps in the wrong order!
WRONG: I've split the o-grid --> fine I've tried to extrude faces before I've associated the edges to curve of small pipes WORKING VERSION: I've split the o-grid --> fine I've associated the edges to curves (edges of new faces, generated by splits - curves of pipe) then 'extrude faces' works :):):) I really don't miss any chance to create problems :o. Super!!!! Viele Grüße Lisa |
Perfect Result - but last question
Hello Far,
I got a really good result :)! Could you tell me where the difference is between a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh and b) Mesh > Compute Mesh > Volume Mesh > Hexa-Dominant > Compute I will need a volume mesh which I can import in OpenFoam. OF makes a volume rendering with help of cell points. That should happen after correct conversion from, for example, a volume fluent mesh to OpenFoam. The volume rendering in OpenFOAM fails because the cell points are missing. Maybe I create the mesh in ICEM in the wrong way. In the Output tab > Solver Setup there are three different Output Solvers listed up that contain 'fluent' in its name: Ansys fluent Fluent_V4 Fluent_V6 Do you know the difference between these solvers? Viele Grüße Lisa |
Quote:
a) right mouse button click on Pre-Mesh --> convert to Unstruct Mesh Ansys fluent |
Quote:
I saw one thread in Openfoam forum, where it is discussed in detail how to export mesh for OF from ICEM. Check it.http://www.cfd-online.com/Forums/ope...-openfoam.html |
Quote:
|
how did you make the blocking?
|
Quote:
2. Cut it in x direction for 3 parts. 3. Cut in y direction for 3 parts 4. Cut in z direction for 5 parts 5. delete blocks. 6. Create 0-block for all. Use 4 faces inlet, outlet, left and right 7. Create 0 block for the main tube. 8. Delete middle part 9. Associate geometry and blocks. Move vertex... |
All times are GMT -4. The time now is 05:59. |