3. Mesh Editor

3.1. How do I remove negative volumes?

If you have tetras then it may not.

The Prism mesher should not allow an inverted element, if an inverted element is encountered, it will generate a message saying that you have an orientation error (basically multiple tetras occupy the same volume). If this happens, the best way to fix this is to merge nodes interactively to try to repair the grid when two nodes are merged, the tetras and tris that become collapsed are automatically deleted. In this way, you can merge out the inverted elements. If there are left handed elements instead of a right handed element, use Diagnostics > Check mesh > Volume orientations to diagnose these elements, you can then say fix to re-order the numbering scheme to right-handed.

Normally, smoothing is not the best method. In the first case, it is not the best option, because if you have a orientation error, it is probably due to too many constraints, and smoothing would rarely help. Merging nodes alleviates the overconstrained case and is a better option. In the second case smoothing really doesn't care about this.

[ top ]

3.2. What are different diagnostics for a tetra/prism/pyramid mesh?

If any elements are reported, an automatic Fix can be attempted, or use Select to add these cells to a subset. Using subset manipulation, and mesh editing techniques, diagnose the problem and resolve it through merging nodes, splitting edges, swapping edges, delete/create elements, etc. For more info see the on-line help (4.2 Mesh Editor -> Edit Mesh -> Edit Nodes/Elements/Edges).

For subset manipulation (mesh display), use the "Display subset - Modify" button in the lower portion of the right hand display column. This will be done automatically if "Select" is picked when prompted after the diagnostic is finished. Usually, one would "Add layer" in the pop up menu, then select "Display options - Solid/wireframe" in the right hand column to get a better visualization of the problem.

Keep in mind that after mesh editing, the diagnostics should be re-checked to verify that no mistakes were made.

• Errors
  • Duplicate elements

    This check locates elements which share all of their nodes with other elements of the same type. These should be deleted.

    Note: the delete in the automatic fix will delete only one of the two duplicate elements, eliminating the duplication but not creating a hole.

  • Uncovered faces

    This check will find faces on a volumetric element that either doesn't touch a surface boundary or another internal face. Usually indicates a hole in the volumetric domain. This shouldn't happen initially. It will most likely occur during manual editing and you happen to delete tetra elements.

    The automatic Fix will cover these uncovered faces with triangles (surface mesh), this may or may not be the proper solution. The user may want to Select these elements first, and decide whether the uncovered faces is a result of missing surface mesh, or a hole. If it is a result of missing surface mesh, the Fix will take care of the problem (re-run the check, and say Fix). If the error points out a hole in the model, the user could try to fix the grid manually by creating tetras or merging nodes.

  • Missing internal faces

    This check will find pairs of volume elements, which belong to different families, but do not have a surface element between the face they share in common. This also shouldn't happen initially. The tetra cutter will detect this problem as leakage. Again this would most likely occur during the manual editing process.

    The automatic Fix will create surface mesh in between these cells.

  • Volume orientations

    This check will find elements where the order of the nodes does not define a right-handed element. The automatic Fix will reorder the mis-oriented elements nodes to eliminate this error.

• Possible problems

  • Multiple Edges

    This check will find elements with an edge that shares more than two elements. Legitimate multiple edges would be found at a "T" junction, where more than two geometry surfaces meet.

  • Triangle Boxes

    This check will find groups of 4 triangles that form a tetrahedron, with no actual volume element inside. This is probably not desired. The best way to fix this problem is to Select this region and merge the two nodes that would collapse the unwanted triangle box.

  • Stand alone Surface mesh

    This check finds surface elements that don't share a face with a volumetric element. These can generally be deleted.

  • Single Edges

    This check will find surface elements with an edge that isn't shared with any other surface element. This would represent a hanging edge; the element would be an internal baffle. These may or may not be legitimate. Legitimate single edges would be where the geometry has a zero thickness baffle with a free or hanging edge.

    Note: If the single edges form a closed loop, i.e. a hole in the surface mesh, the user can select Fix when prompted from thepop up menu. A new set of triangles will be created to fill up the hole.

  • Non-manifold vertices

    This check will find vertices whose adjacent elements' outer edges don't form a closed loop. Usually indicates elements that jump from one surface to another forming a "tent like" structure (refer to the help menu - Edit mesh - Diagnostics - Possible problems - Non-manifold vertices for an illustration)

    This would usually pose no problem for mesh quality but will represent a barrier in the free domain that probably shouldn't be there.

    Note: The automatic Fix for this should only be used if the non-manifold volumetric mesh is only inside the surface mesh that is jumping.

  • Unconnected Vertices

    This check finds and removes vertices that are not connected to any elements

  • Check Orientation

    This checks the direction of the face normal of the displayed (visible) surface elements. This check will indicate any locations where duplicate tetras share the same volume. These errors need to be fixed manually, usually by Clearing a subset, and adding specific elements to it in the location where the Orientation was found. The orientation errors will be displayed in the message window with the location. The user can then use "View - Add marker" and type in the coordinates reported in the message window and the marker name (whatever you call it) will appear in that location. Then, select "Modify" in the subset menu, "Add - Specific" then type in (or paste from the message window) the coordinates in the box and select "Near position." The user then has to fix the Orientation errors by editing the volume elements so that the criss-crossing of elements goes away. This is typically done by merging nodes and/or splitting edges.

    Note that [Diagnostics - Which elements] doesn't pertain to this check

3.3. How do I define periodicity?

This will open up a "Model mesh params" window. Towards the bottom you would find a button to "Define periodicity". Click that button to define rotational or translational periodicity.

• Rotational periodicity requires:
• Base point co-ordinates lying on rotational axis
• Axis direction vector
• Angle of periodicity in degrees
• Translational periodicity requires:
• Offset in global X, Y, Z directions (Dimensional quantity)

For Hexa models, you need to do this additionally inside Hexa.

[ top ]

3.4. How do I define an internal/thin wall?

3.5. How do I input "tolerance" to do copy/mirror/merge of meshes?

• Instead of doing "copy", you should just "move" the domain to do "mirror".
• Save the domain file as new name
• Start a new MED session where read the saved domain file and the original domain file
• See the triangles on the mirror plane
• Use "Edit nodes > merge > Visible (tolerance)" to merge the visible nodes within some tolerance

3.6. There are so many options to do smoothing on structured meshes. Could you explain these?

• Domains: Select/Unselect All or By Volume Families (a list will appear) otherwise Select/Unselect individual domains from the left column beneath
• Methods: These selected methods will apply to all of the domains otherwise select and change the method next to each individual domain listing.
• Only Sorenson Hybrid and Thomas & Middlecoff options are available when Export mode is turned off.
• Sorenson Hybrid: Sorenson methods attempts to maintain node distributions (bunching) near the surface boundaries while improving orthogonality. The Hybrid method could be of two types:
• Hybrid Thomas & Middlecoff: - This method maintains orthogonality between block boundaries (subfaces) so you get a nice smooth transition across subfaces and will maintain first layer height from boundary surface
• Hybrid Laplace: This attempts to improve orthogonality and mesh size uniformity
• Thomas & Middlecoff: This generally tries to maintain orthogonality across boundaries while improving orthogonality
• Laplace: Attempts to give a more uniform mesh size for all selected elements
• Interpolation: This (algebraic) generally improves internal angles
• Hilgenstock Hybrid: Not known exactly what it does. The Hybrid method could be of two types:
• Hybrid Thomas & Middlecoff: - This method maintains orthogonality between block boundaries (subfaces) so you get a nice smooth transition across subfaces and will maintain first layer height from boundary surface
• Hybrid Laplace: This attempts to improve orthogonality and mesh size uniformity
• Face methods: This will apply one of the above methods to subface boundaries while all above options were for volume smoothing.
• Plane smoothing: Smooth certain logical planes (constant index). The actual algorithm will be whatever method is selected, but only smooth the nodes on the logical planes which include Start, End and Increment: e.g. if you select I, Start = 0, End = 20, Increment = 5 would smooth all of the nodes on the logical planes of I=0,5,10,15,and 20 and interpolate everything else in between.
• Unselected domain: Not known exactly what it does
• Settings: Save or load all the parameters set or previously set in this menu.
• Number of iterations: The elliptical smoothing equations are solved numerically, so an iterative differencing scheme is used. The default of 25 iterations is good. There is a maximum residual threshold which is in the Parameters panel as Residual factor
• Expert mode: It gives the user more options for Methods, Parameters, Global Edges and Relaxations for zone and subfaces
• Freeze Bunching Edge: It forces the smoother not to change the node distribution on selected edges during the smoothing process but the nodes could move off from the original edge. Selected edge will change color to yellow.
• Freeze Edge: It will assure the nodes won't move off of the original edge that is selected, but may change the distribution pattern along the edge. Selected edge color changes to purple.
  To absolutely fix the nodes on an edge, you must select Freeze Bunching Edge and Freeze Edge, selecting the same edge for each. Selected edge color changes to red.
• Clear all selections: Clear all domains and constraints on edges, subfaces and zones
• Display Selection Off/On: Subface, Edge and Subface constraints will be displayed.
• Parameters:
• Smoothing:
• Navier-Stokes Rel: See below
• Projection limit: This works for node distributions whose first spacing from the surface is less than the geometry tolerance. I believe the value is a distance normal to the surface in which all nodes in between the surface and this value will be interpolated, giving a more orthogonal mesh near the surface. For Navier-Stokes Rel., this value is actually a factor of the average distance of neighboring nodes.
• Angle: fix vertices on freeze edges: If adjacent edges are frozen (by Freeze Edge command) the shared node of the two or more edges will be frozen if the angle between them is larger than the set value. Normally, there is no case when you would have to change this
• Number of constraint steps: Not exactly known what it does
• Max. multigrid levels: It first smooths a superset of elements, then a smaller subset, and on and on until smoothing occurs on the actual element
• Residual factor: This tells you how much drop of residuals should be there (related to iterations)
• Post smoothing(Single): This will maintain a nice gradient between the cells fixed with Projection limit/Navier-Stokes Rel. (near wall layers) and the layers immediately interior of these
• Surface fitting: It constrains boundary nodes on the actual surface. Otherwise, the original quad faces are used to define the boundary constraint
• Conditional smoothing: This condition will assure that the mesh quality will not get any worse than the original worst determinant value
• Check determinants: It tries to maintain determinant value of all the elements when smoothing
• Check projection at start: This will maintain the boundary constraints during the smoothing process, i.e. the nodes will never leave the surface or curve
• Use projection: Some smoothing steps are performed and then the nodes are finally projected onto the surface or curve
  "Check projection at start" or "Use projection" could conflict with each other in some cases
• Pre-defined mesh: It lets you set distributions much like edge parameters in Hexa. Instead of selecting edges, you select subfaces and all nodes logically perpendicur to those on the surface will abide by the distribution function
• Select direction vector: Normal or User defined vector to define the "perpendicular" distribution direction on a face
• Meshing law/Spacing/Ratio: This behaves like in Hexa. Spacing 1, 2, 1-2 and 2-2 would define the first node spacing from the corners of the subface. You also give the Ratio here
• Subfaces can be selected manually with Select or by boundary family Families. Selecting by family gives the report the number of "elements" in the family
• Extend base subface: It would extend the face through all of the domains
• Global edges:Not much known about this
• Relaxation zones I J K:It gives freedom of movement to the nodes within a certain i, j, k zone and freeze all others within that domain. The domain is selected, then you can define the min. and max. i,j,k.
• Steps for in/decrementing ijk: This is to increment by a certain number when using the arrows to change min and max values. Useful if you have hundreds to thousands of nodes along a particular index direction
• Trans i,j,k: - will move the zone instead of decreasing or increasing the min./max. values. e.g. i min = 2, i max = 4, Trans i of one step will give i min = 3, i max = 5
• Show/Select corner vertices: Not much known about this
• Not much known about the scroll bar at the bottom
• Relaxation subface: It gives freedom of movement to selected subfaces. All other unselected subfaces would be fixed
• All block interfaces: select all interior subfaces
• All boundaries: select all subfaces on an exterior boundary
• By Families: Displays an element number
• Non-relaxation zones/subface: freeze the nodes, all other nodes than in zone or subface would be free to move
• Perform:
• Single: It uses all nodes of selected domains when smoothing the mesh. This works best if the selected domains form a block. It seems to fail if you select domains that form, for instance, and "L" or "T" shape. It is more robust than Global described below
• Global: It uses all nodes of selected domains to smooth the mesh. It also uses phantom nodes immediately outside of the selected domains/zones to figure in the smoothing. It works best if only one or a few connected domains are selected at a time
• Post: It does the smoothing based on quality criterion. Only algebraic interpolation methods are used so that "Methods" or "Face methods" are ignored as well as other smoothing Parameters
• All: Smooth all elements within selected domains
• All exclude violate edges: Nodes along selected violate edges will be fixed. Basically, ignore the violate edges. See below
• Concentrate violate edges: Only use the nodes on selected violate edges in the smoothing process. See below
• Violate edges: It allow nodes along seleted edges to violate or jump off the geometry during smoothing. Sometimes, it's impossible to improve the mesh without slightly violating the geometry
• Violate geometry edge value: This is absolute maximum distance that nodes can be moved away from the geometry
• i,j,k min/max: This is to allow geometry violation of only those nodes within the set index range (partial edge violation). The edge number in the column must first be highlighted.
• Criterion: Normally when you try smoothing for Orthogonality or Warp, most of the time, the Determinant gets worse. You might to juggle between then and the Determinant criteria
• Group bad elements: Not much known about this
• Pre-defined mesh: move nodes to abide by the distribution criterion set in Parameters - Pre-defined mesh

3.7. Why can't ICEM CFD read my tetin files?

awk '{if($0 != "") print}' [input filename] > [output filename]

[ top ]

3.8. Why can't I import the Ansys mesh into Mesh Editor?

The cdb files are generated from within Ansys with the CDWRITE command. The filter would need a cdb file generated with either "all", "comb" or "db" option. The format should be "BLOCKED". The detailed description of CDWRITE command is available in the Ansys documentation.

The import supports the conversion of the following Ansys data:
1. Nodes

2. Elements: (Ref: ANSYS 7.0 doc)
1-49,51-83,86-93,95-109,115-123,126-143,145-150,157-167, 169-178, 180-192, 195

The missing elements are not supported because of the following reasons:
MATRIX50 : A superelement, which in effect can be a set of any number of elements. No equivalent in IcemCFD mesh.
HYPER84 : Has dual order nature i.e. can be either linear or quadratic, depending on key options setting. The current interface does not read the keyopts as of now.
85 : Does not exist in ANSYS 7.0.
INFIN110,111 : Ditto as for 84.
112-114: Non-existent.
CIRCU94,124,125 : Geometry doesn't have IcemCFD mesh equivalents. (Used for circuit simulation.)
ROM144 : Ditto as for CIRCU above. (Used for coupled electrostatic-structural system analysis.)
SURF151-154 : Ditto as for 84.
155,156,168 : Non-existent.
PRTES179 : Ditto as for CIRCU above. (Used to define pre-tension sections.)
INTER193,194 : Ditto as for CIRCU above. (Used for modeling structural assemblies.)
MESH200 : Ditto as for 84.

Note: The interface adds missing midside nodes for quadratic elements, if any.

3. All material properties as defined by MPDATA/MPTEMP commands.

4. Real constant data as defined by RLBLOCK commands.

5. Node and element components as defined by CMBLOCK commands are written out as subsets in the unstructured domain file.

6. Nodal DOF constraints(D), Forces/Moments (F), Surface loads(SF) & Body loads(BF).

During translation to IcemCFD mesh, each unique combination of material id, element type id and real constant set id generates a new family of elements.

The filter can also read the Ansys batch files (but is not recommended) within the following limitations:

The command line for ansys2df is invoked with the following arguments:
-d
not recommended) input file>

Any input filename without the .cdb extension is parsed as a batch input file.

[ top ]

3.9. Why do I get error message for the IGES->tetin translation where IGES file is written from CATIA?

You can probably use the direct interface to Catia which can produce a tetin file without the need of an iges file.

[ top ]

3.10. When I try to convert linear to quadratic tets, why do I get the message like "Angle check failed for node XXXXX, Midpoint XXXXX linearized"?

3.11. Why can't I import a PATRAN grid as a "geometry" into MED while the same can be imported as a "mesh" there?

Workaround: You should first try to fix the uncovered faces here, write back the mesh file and then try to read in this mesh into MED as a domain file.

Remember, unless a mesh has QUAD or TRI boundary elements, it cannot be read as a geometry.

[ top ]

3.12. What is "make Consistent"?

3.13. Why does my element numbering in MED look different than in my solver.

It is important to note, that nodes are also taken into the numbering scheme
Typically, the global numbering scheme works as follows:
Nodes are numbered: x-n,
elements are numbered x-n,
where x is defined in File > Options > Edit Options > Display (Node/Elemindex base value -default is 0), and
where n=#values-x-1 (#values is number of nodes, elements, etc.).
For instance, in the above example,
nodes would be labeled 0-909
BAR_2s would be labeled 0-239
HEXA_8s would be labeled 0-647
QUAD_4s would be labeled 0-485

To make everything unique, use Edit Mesh > Edit elements > Renumber
This forces nodes, and elements to all have unique numbers.
This would then influence a global numbering scheme that is different than the local numbering scheme. For instance:
The local numbering scheme would still be similar to above, but the global numbering scheme for the example above would be as follows:
Nodes labeled 0-909
QUAD_4s would be labeled 910-1395
HEXA_8s would be labeled 1396-2043
BAR_2s would be labeled 2044-2283

The best way to see the node/element numbering is with the following tools:
Display Options > Element Numbers will show the global numbering of the elements
Display Options > Node Numbers will show the node numbers (notice the global and local node numbers always stay the same).
To see a local element, vs. a global element, use subsets:
Display Subset > Modify > Clear
Display Subset > Modify > Add:Specific in this form, you can put an element number in the entry to the right of Add by Number, and turn on local or global, if local, you have to define what kind of element you are looking for. Then hit Add by Number. This will display this (these) elements with this number on the screen (You may have to Orient > Home to see it).

[ top ]

3.14. Why I cannot switch off surfaces sometimes?

3.15. In my surface mesh, I found feather edge (bad surface (triangle) mesh, especially in the complicated geometry, the quality of surface mesh is not good. The cell equiangle skew is larger than required. The relative low quality might lead to unstable or divergency in calculation. What's the remedy then?

• you would go to Advanced options in the "Smooth" panel and switch on "Laplace smoothing" there. Accept and close that panel
• Since this works only for boundary triangles, you should turn the TETRA_4 elements to float. Give 2 iterations for quality 0.3. Press smooth to smooth the surface mesh.
• Then you need to smooth your volume mesh. To do this, switch of laplace smoothing, turn TETRA_4 to smooth and then do the normal smoothing you do.

3.16. Some of the CAD->Tetin translators in "Import Geo" require the CAD system installation. Which ones are those?

• UG->Tetin (works with default environment variables)
• Capri->Tetin
• I-DEAS->Tetin (requires SDRC_INSTL to set for SDRC installation directory)
• ProE->Tetin (requires PROE_EXEC_PATH to be set for ProE launching path)
• Cadds->Tetin (at least CV-DORS is needed)

3.17. How do I work through Y+ adjustment tool? Can you tell me step by step?

• Inside MED, when you go to Output > Y+ following form will come up.

  

  Target Value -- Your target Y+ value

  Load Y+ From -- You can load the Y+ value directly from a solver result file or one of the ascii files you made. If you load from a solver result file, then the value of Y+ must be given on either all cells (0 for those cells that don't make any sense), all nodes (0 for all nodes that don't make any sense), or on all face elements. This will need to be tested with a variety of results from different solvers. If you load it from a 'map' file, then the ascii file should contain a map between the node (or face element number) and a y+ value.





• The form you fill in for the map option is shown in the following figure

  

  Type in the file name for the map file along with the offset to the first vertex number. For star, this is 1 because star vertex numbering starts at 1 (as opposed to 0).
  
  

• Select what the Y+ result refers to in the main panel as in first figure. Either it refers to cell results, node results, or is a map between surface node numbers and the y+ node.
  
  

• Execute a script to produce your output file in the main panel. This will execute the script specified. Warning: This will delete the result file first before running the script. If the file isn't recreated, then it knows the script failed.
  
  

• Specify if you want to run the standard or the post smoother in the main panel.
  
  

• You can change the preferences for Y+ algorithm, or the moving mesh algorithm. The picture of those forms are shown in the next two figures.

  

  
  
  

• Select the surfaces, curves and points that Y+ is to be taken from. In this example, prescribed points are added to the corners. Then WALL1, WALL2, WALL3, WALL4, CUV, and POINT all are selected as "Y+ Surfaces" (better named Y+ entities). It needs to know this so it can priviledge the nodes above them as the nodes that should be adjusted with the correction.
  
  

• A portion of the example is shown in the next two figures. The result of running is shown in the final one. The target Y+ value was 50.

  

  

• Figures out what how to get the Y+ value (result file from solver, a map file, values specified on cells, nodes, or surface nodes refering to the Y+ node above it)
• Figures out how far to move the node to match Y+ and multiply this distance by the relaxation constant. Y+ simple linear interpolation.
• Since we want all nearby nodes Y+ nodes to be moved similar distances do the following -- every Y+ node is moved down the average of all of it's Y+ node neighbors. It solves this equation by iteration until the average change of distance is less than .1%.
• Set the Y+ node movement distance as a boundary condition to solve laplaces equation to determine all other node movements
• Run the smoothers specified after each successful movement.

• The post smoother might also smooth out the differences in how far different regions move because of differing Y+.
• Post smoother puts up a little interrupt widget but it isn't removed once it is finished -- only on the next time I start the post smoother.
• We could only test a limited portion of this code. In particular we could not test the direct result from a result file nor did we test the execute file option to create a new result file.
• Not sure what the relaxation value should be. Default is .5 -- but we are thinking it should be more like .7.

• Is it possible to straight away read in the STAR-CD *.pst-file?
  - No. The .pst file format is internal to STAR. You must either create a map file or emit a domain file. If you do the later, we should verify if we can understand the Y+ result in the domain file. Looks like the domain file does handle Y+ in some fashion. Still we need to test this out but in principle the code can handle the domain file from prostar.
  
  
• What's the meaning of the field "backend" in the Y+ Adjustment Tool?
  - The backend reader to read the result file specified for Y+. The variable to read must also be specified.
  
  
• What is the "use specified reader function" for?
  - This is reserved for future use. The idea is to allow the user to define a tcl function that can be used to read their map file. But it probably will be better if I simply remove this GUI entry for now until the interface is available.
  
  
• Since I don't have specific knowledge about this new feature I would very appreciate if you could explain me step for step what I have to do in case of the adaption with STAR-CD (completed with some explanations and recommendations)
  - See in the beginning of this page about how to do the setup. The background is as follows:
  The feature is still somewhat in the development stage. The code works by computing a 'node movement' for all Y+ nodes (ie nodes just above the surface). Movements for all other nodes are then the average of their nearest neighbor. The process of computing the Y+ change is one of relaxation until the maximum amount of movement for all nodes falls below some threshold.
  If your Y+ values are not too far from the target, then the code will probably work because the nodes can be moved without distorting the elements too much. If you are asking for drastic changes in Y+ that really requires the mesh to be refined or coarsened, then at some point it won't be able to satisfy the request because the elements become too distorted.

3.18. How do I stretch or shrink geometry in specific directions?

3.19. How to read INPUT file with named entity data in ICEM?

3.20. Why do I get error message "med.exe has generated errors and will be closed by windows",while trying to smooth mesh to desired quality in mesh editor?How do I get rid of this?

1)Go to the directory where the tetin and domain files are saved.

2)Type the following commands at command prompt to smooth the mesh externally

i)$ICEM_ACN/icemcfd/smooth domainfilename tetinfilename(for UNIX,SGI,Solaris,Linux platforms)

ii)%ICEM_ACN%/icemcfd/smooth domain filename tetin_filename (for Windows)

iii)smooth 0.3 5 no_collapse( here 0.3 represents determinant quality and 5 represents number of iterations for smoothing)

iv)save domainfilename

v)Exit

[ top ]

3.21. I have several geometry files in a directory. I wish that ICEM CFD should take them all one by one, run HEXA using a replay file, save mesh and write output for solver for all of them. Can I do that?

• At this stage, this sort of stuff works only with 4.1.3 type of ICEM CFD directory structure. So, you have to have at least "mesh" and "domains" directory for every icemcfd project,
• This might require some TCL/TK programming,
• Some of the commands may work differently for windows and Unix.

The directory structure which would be used to explain steps here would be:

	med_script.tcl				: Main script file
	input					: to hold all tetin files
	input/tetin1.tin
	input/tetin2.tin
	.
	.
	input/replay.hxa			: Hexa replay file
	icemcfd_projects			: to hold icemcfd projects
	icemcfd_projects/project1/mesh
	icemcfd_projects/project1/domains
	icemcfd_projects/project1/transfer
	icemcfd_projects/project2/mesh
	icemcfd_projects/project2/domains
	icemcfd_projects/project2/transfer
	.
	.

The script file would be run with following command:

icemcfd -batch -script med_script.tcl

Following would be the major lines in your MED script file to do this:

• Some steps behave in a different way on windows and in Unix. So, it's best to define a variable "is_win" on the top and then use that whenever required. Also global environment variable may be needed.

  if { [file exists "/etc/passwd"] } {
    set is_win 0
  } else {
    set is_win 1
  }
  global env
  

• Create the icemcfd projects directory

  if ![file exists "icemcfd_projects"] {
    eval exec mkdir "icemcfd_projects"
  }
  

• Make a loop for all the the cases in the input directory. It should trim ".tin" from the tetin file and the rest i.e. "tetin1" would become the icemcfd project stored in the variable "icemcfd_project".

  set geo_files [lsort -dictionary [glob -nocomplain input/*.tin]]
  foreach geo_file $geo_files {
    set geo_dir [file dirname $geo_file]
    set geo_file [file tail $geo_file]
    set endind [string last . $geo_file]
    incr endind -1
    set geo_name [string range $geo_file 0 $endind]
    set geo_file "$geo_dir/$geo_file"
  
    set icemcfd_project "icemcfd_projects/$geo_name"
    set tetin_file "$icemcfd_project/mesh/geometry.tin"
    set fbc_file "$icemcfd_project/mesh/family_boco.fbc"
    set fluent_file "$icemcfd_project/transfer/fluent.msh"
    set hexa_replay_file "$icemcfd_project/mesh/replay.hxa"
    set mesh_file "$icemcfd_project/domains/hex.uns"
    set output_file "$icemcfd_project/transfer/fluent.msh"
  }
  

• Create the project directory if this does not exist inside this loop.

    if { [file exists $icemcfd_project] } {
      if { [file isdirectory $icemcfd_project] } {
        eval exec rm -rf $icemcfd_project
        eval exec mkdir $icemcfd_project
        eval exec mkdir $icemcfd_project/mesh
        eval exec mkdir $icemcfd_project/domains
        eval exec mkdir $icemcfd_project/transfer
      }
    } else {
        eval exec mkdir $icemcfd_project
        eval exec mkdir $icemcfd_project/mesh
        eval exec mkdir $icemcfd_project/domains
        eval exec mkdir $icemcfd_project/transfer
    }
  

• Copy geometry file and hexa replay into icemcfd project

    eval exec cp $geo_file $tetin_file
    eval exec cp $geo_dir/replay.hxa $hexa_replay_file
  

• Run HEXA

    if {$is_win} {
        mess "win\n"
        eval exec $env(ICEM_ACN)/icemcfd/hexa_batch $icemcfd_project -tetin $tetin_file -i $hexa_replay_file
    } else {
        mess "unix\n"
        eval exec $env(ICEM_ACN)/icemcfd/hexa $icemcfd_project -tetin $tetin_file -i $hexa_replay_file
    }
  

• Load mesh file and define some boundary condition:

    ic_uns_load $mesh_file 3
    ic_uns_set_modified 0
    ic_empty_boco
    ic_boco_solver Fluent_V5
    ic_boco_set LIVE {{FLUID 0}}
    ic_boco_save $fbc_file
    ic_unload_mesh
  

• Write Fluent output file

    set application_run "$env(ICEM_ACN)/icemcfd/output-interfaces/georampant -dom $mesh_file -b $fbc_file -dim2d $output_file"
    if [catch {eval exec $application_run} trans] {
        puts "Fluent translation : $application_run : unsuccessful \n"
    } else {
        puts "Fluent translation : $application_run : successful \n"
    }
  

Hexa replay file: Make sure that it has following type of lines at the bottom:

save_blocking blocking.blk
save hex.uns LIVE proj 2  -family_boco family_boco.fbc

Complete MED replay file would look like:

global env

if { [file exists "/etc/passwd"] } {
   set is_win 0
} else {
   set is_win 1
}

if ![file exists "icemcfd_projects"] {
  eval exec mkdir "icemcfd_projects"
}

set geo_files [lsort -dictionary [glob -nocomplain input/*.tin]]

foreach geo_file $geo_files {
  mess "Handling Geometry: $geo_file\n"
  set geo_dir [file dirname $geo_file]

  set geo_file [file tail $geo_file]
  set endind [string last . $geo_file]
  incr endind -1
  set geo_name [string range $geo_file 0 $endind]

  set geo_file "$geo_dir/$geo_file"

  set icemcfd_project "icemcfd_projects/$geo_name"
  set tetin_file "$icemcfd_project/mesh/geometry.tin"
  set fbc_file "$icemcfd_project/mesh/family_boco.fbc"
  set hexa_replay_file "$icemcfd_project/mesh/replay.hxa"
  set mesh_file "$icemcfd_project/domains/hex.uns"

  set output_file "$icemcfd_project/transfer/fluent.msh"

  if { [file exists $icemcfd_project] } {
        if { [file isdirectory $icemcfd_project] } {
          eval exec rm -rf $icemcfd_project
          eval exec mkdir $icemcfd_project
          eval exec mkdir $icemcfd_project/mesh
          eval exec mkdir $icemcfd_project/domains
          eval exec mkdir $icemcfd_project/transfer
        }
   } else {
          eval exec mkdir $icemcfd_project
          eval exec mkdir $icemcfd_project/mesh
          eval exec mkdir $icemcfd_project/domains
          eval exec mkdir $icemcfd_project/transfer
   }

   eval exec cp $geo_file $tetin_file
   eval exec cp $geo_dir/$geo_name.hxa $hexa_replay_file

   if {$is_win} {
       eval exec $env(ICEM_ACN)/icemcfd/hexa_batch $icemcfd_project -tetin $tetin_file -i $hexa_replay_file
   } else {
       eval exec $env(ICEM_ACN)/icemcfd/hexa $icemcfd_project -tetin $tetin_file -i $hexa_replay_file
   }


   set application_run "$env(ICEM_ACN)/icemcfd/output-interfaces/georampant -dom $mesh_file -b $fbc_file $output_file"
   if [catch {eval exec $application_run} trans] {
     puts "Fluent translation : $application_run : unsuccessful \n"
   } else {
     puts "Fluent translation : $application_run : successful \n"
   }
}

3.22. How do I read a point data file in MED so that I get the points, curves, surfaces automatically?

The simplest syntax of the input point data file could be:

x1 y1 z1
x2 y2 z2
x3 y3 z3
.
.

However, this would create only points and NO curves or surfaces. The reason being, to create these entities an array with row columns should be known. So, to create those entities, the point data file should look like:

m n
x1 y1 z1
x2 y2 z2
x3 y3 z3
.
.
x(m*n) y(m*n) z(m*n)

3.23. While doing smoothing, MED crashes with "Assertion failed: triangle_sizes[i] >= 0.0, file ucurve.C, line 2196 Signal 6 caught!". What is wrong here?

This is fixed in the next version of ICEM CFD. Please contact your nearest support person to get the later (unreleased though) version.

[ top ]

3.24. Does ICEM have the ability to create a Voronoi Mesh?

Currently, ICEMCFD can provide a 3d (tetrahedral) or a 2d (triangular) delauney mesh. The Voronoi mesh would be the opposite or dual of a delauney mesh, where the center points of the delauney mesh would become the nodal points of the Voronoi mesh and vice versa.

We don't currently support n > 4 polygons or n > 8 polyhedras.

3.25. How is the expansion ratio for linear progression calculated? (given number of layers, total height and initial height)

The formula to calculate the expansion ration is given below. 

This will be useful in dealing with extrusion with a certain expansion.

Height of the nth layer from the surface = h[1+(r-1)(n-1)]
                        
                                         = [h(2-r)]+[h(r-1)n]...(after rearranging)

where,

"h" represents height of the first layer
"r" represents the expansion ratio

If number of required layers is N and total height is T. Then,

T = [h(2-r)]N + [h(r-1)]{N(N+1)/2}...... Sum of first N natural numbers = [N(N+1)]/2

Solving for expansion ratio r,

r = [2T + N(N-3)h] / [N(N-1)h] 


Above formula gives the expansion ratio based on initial(h),total height(T) 

and number of layers(N).








[ top ]
 

3.26. Why does my tetin file take too long to load?
If you think your tetin file is relatively small let's say 5-10Mb and it takes several minutes or even hrs to load, first check for the comments in your tetin file. Till version 4.2.2, everytime you save the tetin file a comment starting with "//" comes towards the top of the tetin file. These comments can be quite a lot and could slow down reading of tetin files. This behaviour is gone in the next upcoming version of ICEMCFD.






[ top ]
 

3.28. How do I extrude mesh by using a function for spacing?
The function must be typed in using tcl/tk syntax.  The only recognized variable is "layer" which is the integer number of the layer and will have a sequential value of 1 -> n (number of layers) as the extrusion progresses.  Typical expressions for spacing would be:

Linear progression:

H*(1+(layer-1)*r) where H is the first layer height and r is the expansion ratio (e.g. 0.2)

Exponential progression:

H*power(R,(layer-1)) where R is the expansion ratio multiplier (e.g. 1.2)






[ top ]
 

3.31. Why can't I merge nodes near a quad-ring
Shell mesh can be locked to prevent the automatic functions like Smooth and Remesh from damaging critical mesh patterns.  When Quad rings are generated, these elements are automatically locked.  

You can see which elements are locked by using the Locked Elements Display option under Mesh => Shells in the model tree.  

You can unlock them with Move Nodes => Lock/Unlock. 

After Unlocking the elements, you will be able to merge the nodes.

The next patch should allow locked elements to be manually edited and only prevent automatic editing functions.






[ top ]
 

3.32. When I try to change the curve mesh size, why do I get the following error: "Warning: Using automatic sizing;...using xxxx for global mesh size"?
The global max element size is set automatically in case it is undefined and there are no (or inadequate) element sizes given on curves and surfaces.  The automatic size is based on various geometry dimensions and depends on the selected meshing option.  It provides a good average choice for meshing.







[ top ]
 

[ top ] [ previous ] [ next ] 

created by faq-system 0.3.6 Thomas Linden