|
Zhou Bin,
blockMesh is suit
Zhou Bin,
blockMesh is suitable for simple geometries, which yours is not. However, in about an hour I drafted an example of your mesh using Blender and Calculix. Example images and file are attached. I did this simply to see if my technique works for your kind of geometry, which it does. See the following URL for an overview of the technique: Outline of method Example Surface: http://www.cfd-online.com/OpenFOAM_D...your_image.gif Image of surface mesh: http://www.cfd-online.com/OpenFOAM_D...your_image.gif The Blender file: I would expect you'd need a few days to learn Blender and a day for Calculix, but this would be more rewarding and likely faster than trying to use blockMesh. Good Luck, Doug |
Zhou Bin,
blockMesh is suit
Zhou Bin,
blockMesh is suitable for simple geometries, which yours is not. However, in about an hour I drafted an example of your mesh using Blender and Calculix. Example images and file are attached. I did this simply to see if my technique works for your kind of geometry, which it does. See the following URL for an overview of the technique: Outline of method Example Surface: http://www.cfd-online.com/OpenFOAM_D...ges/1/5588.jpg Image of surface mesh: http://www.cfd-online.com/OpenFOAM_D...ges/1/5589.jpg Image of how you construct the mesh: http://www.cfd-online.com/OpenFOAM_D...ges/1/5590.jpg The Blender file: http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif barWithHoles.blender.tar.gz I would expect you'd need a few days to learn Blender and a day for Calculix, but this would be more rewarding and likely faster than trying to use blockMesh. Good Luck, Doug |
Zhou Bin,
blockMesh is suit
Zhou Bin,
blockMesh is suitable for simple geometries, which yours is not. However, in about an hour I drafted an example of your mesh using Blender and Calculix. Example images and file are attached. I did this simply to see if my technique works for your kind of geometry, which it does. See the following URL for an overview of the technique: Outline of method Example Surface: http://www.cfd-online.com/OpenFOAM_D...ges/1/5593.jpg Image of surface mesh: http://www.cfd-online.com/OpenFOAM_D...ges/1/5594.jpg Image of how you construct the mesh: http://www.cfd-online.com/OpenFOAM_D...ges/1/5595.jpg The Blender file: http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif barWithHoles.blender.tar.gz I would expect you'd need a few days to learn Blender and a day for Calculix, but this would be more rewarding and likely faster than trying to use blockMesh. Good Luck, Doug |
Dear Doug,
Really thank you f
Dear Doug,
Really thank you for your seggestions, because my geometry is really complex and I think I may have difficulty in meshing. Now you help me a lot, and I'd like to see if we can mesh using Blender and Caululix. Best regards Zhou Bin From Politecnico di Torino |
Dear Doug,
I have learned Ble
Dear Doug,
I have learned Blender for several days, and it is really powerful, thank you for introducing it to me. Now as far as I know, we first create a basic geometry and then to edit the object. In the above method you tell me, I should use the Blender function "subsurf", and use only squares for the surface. But at first there's no objects yet, I could not choose "subsurf". Since I do not know how to create a rectangular with about 100 circles in Blender first. I only have these data (coordinates and diameters), could you explain it to me? If possible, could we talk in MSN? Thank you. Sincerely, Zhou Bin (MSN:zhoubinwx"hotmail.com) |
Zhou Bin,
I'd take the foll
Zhou Bin,
I'd take the following steps... 1) Create a square centered at (0,0,0) with sides of dimension = 1. (Press "N" to see Transform Properties). We will use this square as a template http://www.cfd-online.com/OpenFOAM_D...ges/1/5666.jpg 2) For each circle, copy this object (shift-D); scale by diameter ("S", then type in the number); and move it to the proper location by typing its coordinates into Transform Properties. Below you will see your first circle as the active object, and the template at (0,0,0). http://www.cfd-online.com/OpenFOAM_D...ges/1/5667.jpg 3) After repeating (2) above for each circle, you can delete your template. Now, select all the objects and join them (control-J). I've accomplished this for our first three circles as shown below in Edit Mode. You will need to press the Tab-key to enter Edit Mode. http://www.cfd-online.com/OpenFOAM_D...ges/1/5668.jpg 4) You'll need to delete all the faces while keeping the points and lines. To do this, select all points as is shown in the above image, then press "X" and delete "Only Faces". Now, you need to fill in all of the surfaces on your rectangle. For the example here with only three of your holes it is rather easy. As you add more circles of various dimensions you will need to use judgment to achieve the mesh density you desire. So, I'd select the lower vertices on the three squares, press "E" and select "Only Edges" to extrude the lower edges as shown below. http://www.cfd-online.com/OpenFOAM_D...ges/1/5669.jpg 5. The above image shows that the cursor is located at (0,0,0). Also, in the bottom of this image you will see the words "Edit Mode". Two spaces to the right of these words you will see that the 3D-Cursor is selected as the Pivot. From here, you can scale the selected vertices down to the Cursor by pressing "S" for scale, then "Y" for scaling parallel to the y-axis, then the number "0" to scale down to Cursor. http://www.cfd-online.com/OpenFOAM_D...ges/1/5670.jpg 6. Next, I've done the same extrusion in the y-direction. Notice that I've closed the Transform Properties box since we really don't need it at this time. http://www.cfd-online.com/OpenFOAM_D...ges/1/5671.jpg 7. Now, fill in the faces between the holes by selecting each group of four verticies anf pressing "F". One of the faces is shown below. http://www.cfd-online.com/OpenFOAM_D...ges/1/5672.jpg 8. After adding all the faces we have the following shape. http://www.cfd-online.com/OpenFOAM_D...ges/1/5673.jpg 9. Now extrude the upper edges to y=75 for the top of your bar. By now, you will have the technique from (1) through (8) above. http://www.cfd-online.com/OpenFOAM_D...ges/1/5674.jpg 10. Then extrude the right side to x=430. At this point you have the bar shown below with three tiny holes. The lower panel of the image below is the Buttons Window. By pressing function key "F-9" you will be in editing options mode for the selected object. The selected object is your pink highlighted rectangle in the upper panel. To the far right of this editing options panel you will see the Modifiers tab. Click "Add Modifiers" to then select "Subsurf" from the list. You can increase your surface mesh density by changing "Levels:" which by default is set to 1. For now, we'll keep this default value. Don't be concerned about "Render Levels"; this is only used when you want to make a nice rendering of your object. http://www.cfd-online.com/OpenFOAM_D...ges/1/5675.jpg 11. By zooming into a view of the three holes and pressing "Z", you will see a wireframe of your mesh beginning to take shape. http://www.cfd-online.com/OpenFOAM_D...ges/1/5676.jpg 12. A nice feature of subsurf is that by default all the sharp edges of your object become beveled. This default feature has converted the square holes into circles. But sometimes, you'd like the edges to remain in place, like the edges of your rectangle. We need to select the edges of the rectangle and crease them. You'll see in the lower part of the next image, to the far right of the words "Edit Mode", a depressed button that looks like a slash "/". In this selection mode, only edges can be selected. I've selected all the edges on the perimeter of the rectangle (highlighted in yellow below). Then, by pressing "shift-E" followed by the number "1", these edges are creased. http://www.cfd-online.com/OpenFOAM_D...ges/1/5677.jpg 13. We're nearly done. Tabbing back into object mode we now have the coarse wireframe image. You may have noticed that the far right hole has a pink dot at its center. That dot was the origin of that square back in step (2). When we joined the objects in step (3) above, this became the origin of the joined object. We need to move the object origin to (0,0,0). In edit mode, select only the vertex at (0,0,0), press "shift-S", and then select "Cursor->Selection". This will snap the cursor to the selected vertex. Now, in the lower panel of the image below, we have Edit Options with several tabs. Under the "Mesh" tab you will see the "Center Cursor" button. Press this button, and the object origin will move to the cursor location. This step is much easier than it sounds. http://www.cfd-online.com/OpenFOAM_D...ges/1/5678.jpg 14. Increase subsurf levels, say to 3, and you will have a more refined surface grid as is shown below. If you need more control of the grid in the neighborhood of each hole, you can extrude a square around each object of (2) above before you perform the join of step (3). I gave an example of a this kind of surface with grid control-points around each hole in my original post to this thread. http://www.cfd-online.com/OpenFOAM_D...ges/1/5679.jpg Beyond this, there are many excellent tutorials for Blender available on the internet. Just search "Blender tutorial", or go to the blender.org website. Enjoy, Doug |
Dear Doug,
Really thank you f
Dear Doug,
Really thank you for your detail steps, we are trying now, since we'll have many models of this kind, in your step 2, we repeat to input the circles information, well, as for us, it is labor consuming for many such models. Do you have any good solutions for this problem? By the way, since we could input and scale the circle by hand, could we use code in Blender or not? Because I'm new, I appreciate your great patience to read my problem? |
Zouh Bin,
Blender has a Pyt
Zouh Bin,
Blender has a Python API, useful for data import/export. At "Outline of Method" in my original post to this thread is a Python Script for exporting to Calculix FBD format. You could perhaps develop a similar script to import your data. Blender includes many data import/export scripts which you may want to study. Doug |
Zhou Bin,
Very nicely done.
Zhou Bin,
Very nicely done. I trust you used some simple program to generate the list of points. After executing the Python script you created, set the subsurf level=2 (See step 10 above) and while in Object Mode press the "Apply" button next to the subsurf levels. This permanently subdivides each circle into sixteen faces with nine interior verticies. Tab-key to Edit Mode, and for each circle select the nine interior verticies, press the X-key to bring up the delete dialogue, then select verticies to delete the selected verticies. You now have sixteen verticies defining the edge of each circle. This is both good and bad news. The good part is that you have finer control of how the mesh is constructed, while the bad part is you have more lines to manually generate. Given the complexity of your object, this may be more good than bad. After you have created all the faces, you can again modify with subsurf (Step 10 above) to refine the surface grid. To simplify your work, you could seperate from your mesh an object containing only those circles that need refinement, apply the subsurf to those seperate circles, then rejoint your two objects. You'd then have some circles with sixteen points and others with four points. I'm on travel and away from my workstation so am unable to create mini-tutorial for you, but you should be able to find a seperate/join Blender tutorial on the internet. This approach will work. You could also create your object directly in Calculix using curved lines, but in my opinion the Blender interface is much easier to use and provides much higher functionality. Doug |
Zhou Bin,
Better answer is
Zhou Bin,
Better answer is as follows. After you create squares using your Python script, select Mid-Point as your Pivot. (Step 5 above shows how to select the Pivot.) Now, you can select the four verticies of any of your squares and rotate about its mid-point by pressing the "R" key. From what I see of your geometry, you should be able to avoid overlaps by simply rotating neighboring squares. If you still have an overlap, you can seperate that one square from the object, apply the subsurf, then join the two objects together again. This way, most all of your circles will be defined by only 4 points, which reduces the number of faces you'll need to manually create in your surface mesh. You may find after working with this you'd like to apply subsurf to your larger circles, and keep all of your smaller circles at just 4 verticies. My guess is that this approach will help keep all of the cells at a similar size. Doug |
Dear Doug,
I have tried your
Dear Doug,
I have tried your suggested way, and I find after I run the script, I can only select all the circles, but not one by one, so I can not rotate; As I say, in my model I need to link a lot of vertex, which is really time-consuming. I have several this kind of models, not only this one. Therefore, would you please give any suggestions about linking vertex automatically? I'll think about this during your travel. Wish you a happy weekend. Best regards, Zhou Bin |
Zhou Bin,
Your question now
Zhou Bin,
Your question now is regarding basic Blender functionality. There are many, many tutorials available on the internet about how to mesh an object in Blender. As for selecting an individual circle, first select the object which of course will highlight the entire object. Then, press the Tab-key which will toggle you between object mode and edit mode. Once you are in edit mode you can select/edit/add/delete/manipulate individual vertices within the object. As for linking the circles, I've always found in Blender that I prefer to manually build up the surface because I can then control precisely the size and shape of each face of my surface. An automatic method is available for what you want to do. You can create a second object which is your rectangular bar without any holes, then boolean subtract your Circles Object from the Rectangle Object. You may want to apply subsurf to some or all of the circles in your Circles Object before you boolean subtract it from your Rectangle Object. I would suggest that if these instructions are unclear that you walk though several Blender tutorials and then re-read these instructions. After you are accomplished at object mode, edit mode, subsurf, vertex manipulation, and boolean operations, and you still have questions I would be happy to help further. You have many, many advanced methods in Blender to create and modify your surface mesh, including smoothing functions, converting triangles to squares (or vice versa), removing faces, subdividing faces, etc. , but you first need to teach yourself the basics. Doug |
Dear Doug,
Now I'd like to ou
Dear Doug,
Now I'd like to output the geometry, the data file named "holes.txt"containing the coordinates and diameters: 0 0 430 0 430 75 0 75 44.69 60.83 5.93 100.24 55.18 2.53 72.4 26.52 5.6 389.86 31.52 5.87 169.69 25.04 4.63 383.35 7.28 5.87 35.88 36.69 1.59 181.73 49.3 1.21 283.25 11.04 3.1 16.86 1.61 1.46 156.68 64.18 10.29 200.65 22.23 4.76 321.28 38.1 5.51 2.75 23.87 2.9 332.09 53.86 5.26 359.66 48.71 12.22 5.93 17.32 6.32 78.12 72.39 5.12 220.93 65.76 5.76 115.37 36.68 4.7 112.42 61.96 1.17 57.63 51.96 3.61 240.5 4.66 3.03 242.86 63.09 3.07 230.74 16.71 1.4 |
Well, dear Mr. Doug, do you ha
Well, dear Mr. Doug, do you have any comment on my current situation?
Now I begin to mesh this geometry in Calculix, for my complex geometry, I do not know if it is difficult to mesh. I'll study hard on Calculix, Thank you. Best regards, Zhou Bin |
Zhou Bin,
You need to attac
Zhou Bin,
You need to attach the script so I can open the file with proper formatting. Cut and paste will not run. See "Formatting" under "Documentation" in the left frame of this webpage for instructions on how to attach a file. I'd like to see the working script. If it produces a surface mesh that you are happy with, you are very nearly done. Doug |
Dear Doug,
Thank you for your
Dear Doug,
Thank you for your post. Now let me try to upload the files, please check. The Blender file is: http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif holes.rar and the txt file is: http://www.cfd-online.com/OpenFOAM_D...s/mime_txt.gif holes.txt Zhou Bin |
Dear Doug,
It works for me to
Dear Doug,
It works for me to upload files,very interesting, thank you. Best regards, Zhou Bin |
Zhou Bin,
The file opens an
Zhou Bin,
The file opens and I am able to see the surface mesh you have. I would not be satisfied with this mesh because it has lots of very long lines bunched together, and then very large surfaces in other areas. I doubt that any volume mesh extruded from this surface would pass the OpenFOAM checkMesh utility without errors. Your automated method is very well done but inappropriate I think, sorry. You need to have a clear understanding of what you want your final mesh to look like. The manual method I suggested above with four points per circle is labor intensive, but in a day or two you'd likely have a good mesh. If you were to start with Calculix, you still have the same issue of connecting your circles in a way that generates a useful surface mesh. The Blender interface is very sophisticated and more productive for this kind of task, which is why I use it and then export to Calculix. Doug |
Dear Doug,
Your suggestion se
Dear Doug,
Your suggestion seems quite reasonable. My aim is like: http://www.savefile.com/files/1159333 I really thank you for you encouragement. I will go ahead, and by the way, would you please give me any suggestion after you see the attached pictures. Best regards, Zhou bin |
Zhou Bin,
Calculix only sen
Zhou Bin,
Calculix only sends hexahedral elements to OpenFOAM. The image has tetrahedral elements. Netgen, an open source tool, might work for you with tetrahedral. I work exclusively with hex which I understand to be preferred for fluid analyses even though tets will sometimes work. If you need a hex mesh at the boundary layer of the circle and then want to fill the open spaces with tets, you can use your python script with Blender/Calculix to create the boundary layer mesh, and then possibly use Netgen to fill in the open space with tets. OpenFOAM has utilities to then merge and stitch two meshes together. I've considered this approach but did not persue because pure hex has worked for me in Blender/Calculex even for rather complex surfaces. If you need automated meshing for many cases, then tets with possibly hex at the boundary layer could be a productive approach. Search this forum for "cylinder" and you will find some nice images of hex at the blundary layer and tets in the open space. As I recall, the forum also has postings on "Netgen" for exporting tets to OpenFOAM. Doug |
Dear Doug,
Since I have only
Dear Doug,
Since I have only several days to finish meshing, I would like to accept your advise, using hex for my case. I'll let you know my progress. Thank you. Zhou Bin |
Dear Doug,
I am really impr
Dear Doug,
I am really impressed by the capabilities of Blender and Calculix together and I would like to start using them as meshing tools. Before starting, I have a couple of curisosities about them: 1) Are you using them for only 2d meshes or also 3d? 2) Which kind of geometries are you modelling? 3) Could you post a couple of images of some meshes? 4) What about the mesh quality (skewness/non-orthogonality)? Thanks a lot, Bye Tommaso |
Doug,
I forgot the last qu
Doug,
I forgot the last question: have you ever tried meshing STL surfaces with Blender? Thanks again, Tommaso |
Dear Doug,
When I install Cal
Dear Doug,
When I install Calculix, and go ahead one by one according to the installation, but at step 8, after I type: cgx -b dummy.fbd. the system tells me that: the input file dummy.fbd can not be opened. I stop here and have done this for two days. Kindly, Zhou Bin |
Tommaso,
Q1) Are you using
Tommaso,
Q1) Are you using them for only 2d meshes or also 3d? A1) Blender for 2-D compound curve surface, then extrude in Calculix for 3-D external flow. Q2) Which kind of geometries are you modeling? A2) Concave/convex surfaces, beginning to use what has been called manifolds for joining multiple meshes. The Python tool I posted in a separate thread works great for external flow over uniformly convex bodies of revolution. Q3) Could you post a couple of images of some meshes? A3) Everything I have done is private. I'm currently working overtime on one project. Perhaps in the next month I'll have free time to create a public example. Q4) What about the mesh quality (skewness/non-orthogonality)? A4) For highly curved surfaces where extrusion is not orthogonal, I can pass all meshCheck except nonOrthogonal warnings. I must iterate between Blender/Calculix/OpenFOAM to achieve this quality, and its becoming faster for me so that maybe in about 4-5 iterations I have a high quality mesh. Also, subsurf in Blender has generated one or two warped surfaces warnings. For flat surfaces with orthogonal extrusion, no errors or warnings. Q5) STL? Q5) I once imported an STL into Calculix, extruded it, then meshed it with hex. Looked kinda funny, even passed meshCheck, but I didn't run the solver. Blender has the ability to import/output an STL, which I have used on occasion as a template for creating a subsurf with square elements. I prefer square and hex. Doug |
Zhou Bin,
> input file dumm
Zhou Bin,
> input file dummy.fbd can not be opened. This is correct. Calculix needs a filename to start running. If you then create geometry in Calculix and Save, your geometry will be saved in dummy.fbd . This and more is covered in the tutorial that is provided with Calculix. Doug |
Dear Doug,
Here we have a fes
Dear Doug,
Here we have a festival in Italy, so I'm sorry I could not reply you immediately. Now I can see that this is not a problem, and I can go ahead. Thank you. By the way, the geometry you post entitled " Image of surface mesh" is quite well, and I'd like to use this way, but afterwards you post on Saturday, October 13, 2007 - 12:11 pm, the mesh is different. Because at first the circle is made from rectangle, How you make another rectangle around the circle for mesh in your first case? Or just like the usual way? |
Dear zhoubin,
are you worki
Dear zhoubin,
are you working with OpenFOAM and Blender in Italy? Is it possible to know which is your company/university? Thanks a lot, Tommaso |
Dear Tommaso:
I am a student
Dear Tommaso:
I am a student here in Politecnico di Torino, nice to meet you. Best regards, Zhou Bin |
Zhou Bin,
Good. The square
Zhou Bin,
Good. The square around the square allows you to control the mesh at the boundary of the circle. That too is the way I'd do it. The simple technique is to set the Pivot to Midpoint, in Edit Mode select one square, then press the "E"-key to Extrude. Press <escape> so that the extruded square keeps the same dimensions as the original square, then press the "S"-key to scale the square about the midpoint pivot. I'm on travel through mid-next week. You should be able to locate a tutorial on Extrusion. The one trick not usually taught is <esc>, then S-key to scale the extrusion. Doug |
Dear Doug,
First have a nice
Dear Doug,
First have a nice trip. I'll show you what I have done during your trip next week. Best regards, Zhou Bin |
Dear Doug,
OpenFOAM has a p
Dear Doug,
OpenFOAM has a period of no function, and between this time, I have posted my current situation here. Now, I want to tell you that I have solved the problem of 4 z just as you said. Really thank you. After I select the boundary with the command qadd and qrem, I have many files, however, in the 4 files: boundary, cells, faces and points, I could not find the boundary I selected. But in the files I saved, which is named as "holewithin.fbb". Do you generate the file "boundary" which can contain the selected boundary? Best regards, Zhou Bin |
Dear Doug,
in the parent di
Dear Doug,
in the parent directory of project, I input: checkMesh .project, but an information tells me: FOAM FATAL ERROR:Wrong number of arguments, expected 2 found 1. I don't know if you have this kind of problem or not? Best regards, Zhou Bin |
I check the mesh from Calculix
I check the mesh from Calculix to openfoam, but I get the following information:
root@openfoam:~/OpenFOAM/root-1.4.1/run# checkMesh .filter /*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.4.1 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : checkMesh .filter Date : Nov 19 2007 Time : 14:17:22 Host : openfoam PID : 6527 Usage: checkMesh <root> <case> [-parallel] [-fullTopology] [-cellDeterminant] [-pointNearness] [-latestTime] [-time time] --> FOAM FATAL ERROR : Wrong number of arguments, expected 2 found 1 FOAM exiting After several hours check, I still could not find the reason. |
Dear Zhou,
you should run:
Dear Zhou,
you should run: checkMesh . filter and not checkMesh .filter bye |
Dear Tommaso,
Last night I
Dear Tommaso,
Last night I had the same solution like you suggest, this morning I tried, and I got: ---------------------------------- Exec : checkMesh . filter Date : Nov 20 2007 Time : 08:00:07 Host : openfoam PID : 5462 Root : /home/zhou/OpenFOAM/root-1.4.1/run Case : filter Nprocs : 1 Create time --> FOAM FATAL IO ERROR : cannot open file file: /home/zhou/OpenFOAM/root-1.4.1/run/filter/system/controlDict at line 0. Function: regIOobject::readStream(const word&) in file: db/regIOobject/regIOobjectRead.C at line: 66. FOAM exiting ------------------------------------ I'm searching and thinking about this problem. Best regards, Zhou Bin |
Dear Tommaso,
I have solved t
Dear Tommaso,
I have solved this problem, and I would like to post it here, hope it is useful for others: I copy controlDict from icoFoam, then I change some parameters inside use "gedit ..." Now it is ok. Best regards, Zhou Bin |
Dear Doug,
I am very glad t
Dear Doug,
I am very glad to tell someone else who has the similar model with me that: after I use gmsh for meshing, I am impressed by the power of gmsh---- a powerful tool with simple platform. I could control the mesh around each circle very easily and mesh them for one click. Sincerely thank you for introducing me Blender for a long way. Best regards, Zhou Bin |
| All times are GMT -4. The time now is 13:44. |