Chapter 5.1 Mesh Preparation and Output to Solver ICEM CFD Introductory Course

Edit Mesh Usage of Edit Mesh tools To diagnose and fix any problems and improve mesh quality To convert element types Refine and/or coarsen mesh Manual and automatic tools For imported as well as internally created mesh

Mesh Checks To diagnose mesh associativity problems Errors – most likely to cause problems in: Solver translation Solver input Solution convergence/run Possible Problems – “Unclean surface mesh” Unwanted elements Unwanted holes/gaps May result in incorrect solution Can check any combination of errors/possible problems at any one time Individually select Click on Error or Possible Problems tabs will select all options in column – selecting again will de-select all Set Defaults will select most commonly seen/detrimental diagnostics Check Mode Create Subsets – creates a subset of elements that fit each criteria Check/Fix Each – offers automatic fixing of indicated problem

Mesh Checks: Mesh Errors Duplicate Elements Elements that share all nodes with other elements of the same type Uncovered Faces Volumetric element faces that are neither attached to the face of another volumetric element nor to a surface element (boundary face) Missing Internal Faces Volumetric elements that are adjacent to another of a different part with no surface element between them Periodic Problems Inconsistency in the number of nodes/faces between periodic sides Special check for rotating (sector) or translational periodic grids Volume Orientation Left handed elements due to incorrect connectivity (node numbering of cell) Surface Orientations Volume elements that share the same surface element (overlap) Hanging Elements Line (bar) elements with a free node (node not shared by another bar) Penetrating Elements Surface element(s) that intersect or penetrate through other surface elements Disconnected Bar Elements Bar elements where both nodes are unattached to other bars

Mesh Checks: Possible Problems Multiple Edges Surface elements with an edge that shares three or more elements Can include legitimate T-junctions Triangle Boxes Groups of 4 triangles that form a tetrahedron with no actual volume element inside 2 -Single Edges Surface element with 2 free edges (not shared by another surface element) Single-Multiple Edges Surface element with both free and multiple edges Stand-Alone Surface Mesh Surface elements that don't share a face with a volumetric element Single Edges Surface elements with a free edge Can include legitimate hanging baffles Delaunay Violation Tri elements with nodes that are within the circumsphere of adjacent elements legacy quality criteria Overlapping Elements Continuous set of surface elements that occupy the same surface area (surface mesh that folds on to itself) Non-manifold vertices Vertices whose adjacent elements’ outer edges don't form a closed loop Typically found in tent-like structures where surface elements jump from one surface to another across a narrow gap or sharp angle Unconnected Vertices Vertices that are not connected to any elements Usually eliminated automatically upon saving the mesh

Mesh Checks If Create Subsets was selected Will go through all checked criteria at once Elements that have a particular error/problem are put into a subset with that diagnostic type name Subsets activated in Model Tree Turn off all parts or shells to view subsets If Check/Fix Each was selected Will be prompted with options one criteria at a time Fix: Automatically fix the error/problem Recommended only for Duplicate Elements, Volume Orientations, Periodic Problems, Overlapping Elements Create Subset Ignore For example, multiple edges may be legitimate t-junctions; single edges – legitimate free edges

Mesh Smoothing Automatically improve element quality User chooses: All element types Necessary to have geometry loaded Nodes are moved to improve the element quality Automatic node movement constrained by node projection type to geometry type – e.g. curve nodes will be constrained to move only on curves Histogram is automatically displayed/updated after smoothing User chooses: Criterion Smooth Mesh Type Smooth: Element types actively smoothed; quality of type appears as part of histogram. Freeze: Nodes are held in place during the smoothing process; elements not in histogram Float: Nodes can be moved along with adjacent smoothed elements, but quality ignored; not shown in histogram Example: Freeze Prisms and Pyramids while smoothing Tetra. Float surface elements

Mesh Smoothing Advanced Options Smooth Parts/Subsets Laplace smoothing Smooth all parts, visible parts (activated in model tree), or visible subsets Quick, local smoothing Laplace smoothing Gives more uniform mesh size relative to neighboring elements Recommended for TRI only – smooth Tetra after with Laplace turned off Recommended prior to prism generation Not just worst 1% Factors in all elements instead of only the worst 1% of those beneath quality value and their neighbors Violate geometry Unconstrain nodes slightly from geometry within user defined tolerance – absolute or relative to minimum edge length of mesh elements

Output ANSYS ICEMCFD Allows you to write input files for many CFD and FEA solvers. The output tab can be used to, Select solvers Define boundary conditions Edit parameters Write input file

Wing Edit Workshop File > Change Working Dir… Choose WingEdit OK Use the quick icon to open geometry Choose WingEdit.tin Open

Compute Mesh Select Mesh > Compute Mesh > Volume Mesh Set Mesh Method > Robust (Octree) (default) Compute

Quality histogram after smoothing Mesh Smoothing Mesh Smoothing Edit Mesh > Smooth Mesh Globally Specify 5 Smoothing iterations Up to quality 0.4 Use other defaults Apply Right-click in quality histogram and select Replot to modify its display as shown Quality histogram after smoothing

Reviewing the mesh Quality Histogram Left-click on the columns up to 0.3 in the histogram to select the elements within those ranges Hide Shells from the tree to make the elements easier to find Review curves, and points to determine root cause Extra curves and points in the geometry added additional constraints

Create/Modify subset Using a Subset With the bars up to 0.3 selected, right-click in the histogram and select Subset The elements are placed into a diagnostic subset called Aspect ratio (or selected criteria during smoothing) under the Mesh branch Right-click on the subset name and select Modify Select Add Layer(s) to Subset Add 2 layers with Also volume elements turned off This adds additional elements for ease in seeing surroundings Select Remove from Subset by Selection Click on Select all volume elements from the selection Select mesh elements toolbar To only visualize and edit surface elements Very difficult to view and edit volumes and usually not necessary

Merge Nodes Merging Nodes Edit Mesh > Merge Nodes > Merge Interactive Activate Ignore projection to allow removed node to un-project With the subset displayed, turn off Shells from the tree Right-click on Mesh and select Dot Nodes Select 2 nodes from the screen – the first node is kept, the second is removed Continue for length of problem are (~8 or 9 locations)

After merging and smoothing Mesh Smoothing Mesh Smoothing Always smooth after manual editing Edit Mesh > Smooth Mesh Globally Use previous settings Apply Verify that lowest quality elements are removed from tail area Right-click on the subset name “Quality” from the model tree and select Clear Manual node movement is also possible using Edit Mesh > Move Nodes > Interactive Preserves projection to geometry types Remember to smooth again…. Before merging After merging and smoothing

Check Mesh Checking the Mesh Select Edit Mesh > Check Mesh Use the default set of checks and Apply For Duplicate elements select Fix These are duplicate line elements from the node merging process For Hanging elements select Fix These are Node elements no longer connected after re-meshing the subset For Unconnected vertices select Delete These are normally deleted during the Save process

Select Solver Select Solver Select Output -> Select Solver Select Fluent_V6 as output solver Apply

Define Boundary Conditions Select Output -> Boundary Conditions Expand Volumes Parts that have volume cells are listed here Expand the part LIVE Click on Create New Select the appropriate boundary condition (fluid) from the pop up window Click OK Similarly Expand Surfaces to see the parts that have the shell mesh. These parts could make up the walls, inlet, outlet etc. Expand the parts and define the appropriate boundary conditions Click Accept

Write Input Write input file Select Output -> Write input When prompted, save the project as WingEdit.prj When prompted, open WingEdit.uns mesh file The Fluent_V6 panel pops up The output file will be saved in the working directory. The default name of the file is fluent.msh. The file name and location can be changed by typing it in the Output file filed Click Done. Fluent.msh file is created in the working directory