UW : ERC : Staff : Home : Research :

This page is devoted to making itape17 files with ICEM-CFD

  1. What are the steps for restarting an ICEM-CFD session?
  2. How do I re-mesh a grid?
  3. What are appropriate boundary conditions for kiva3v sector grids?
  4. If ICEM-CFD IJK orientation is not appropriate for kiva3v, how can it be fixed?
  5. How can I change the squish height of an existing mesh?
  6. Can an itape17 be used in ICEM-CFD?
  7. Is there any difference between piston/liner crevice representation in ICEM-CFD grids and those made with k3prep?
  8. What is a technique for getting nice curves on sharp edges?
  9. If ICEM-CFD diagnostics tell me there are Multiple Edges, is that OK?
  10. Are there guidelines for when to use automatic vs. manual fixes?
  11. Should spaces be avoided in directories and file names?
  12. Do you have suggestions for creating an icem-cfd grid from an existing itape17?
  13. What must be done on-axis for sector grids in icem-cfd?
  14. How can I bring up the old icem-cfd interface in version 5?
  15. Is there a way to assign different node counts to parallel edges?
  16. What is needed to create surfaces in hexa?
  17. Why does icem-cfd report different distances when using local coordiante systems?

What are the steps for restarting an ICEM-CFD session?

Reasons a modeler might want to do restart a session are:

  1. Start ICEM-CFD
  2. Select the ICEM-CFD project to open
  3. Select the tetin (geometry) file to load
    If you are in the building geometry stage, you may not have any domain files to load and you can continue building the geometry from this point.  If you do have domain files to load, continue with the next step.
     
  4. Select the domain (mesh) file, or files to load
    Note that it is believed that these domain files should be in the same directory as the tetin file.  In working with kiva, it is likely that you previously created many domain files.  If this is the case, a file called Multiblock may appear as an option.  You can select Multiblock, instead of all of the individual blocks.  If the Multiblock option causes problems, select all of the applicable domain files and when asked if to 'Merge', or 'Keep Separate', choose Merge (for every domain when prompted).
  5. If you also previously assigned boundary conditions, then select File > Open > Boundary condition file and select the correct boundary condition file (ex: family_boco.fbc)

How do I re-mesh a grid?

  1. Perform the steps from What are the steps for restarting an ICEM-CFD session?
  2. Select Meshing
  3. Select Hexa > Interactive
  4. Load in the blocking file that you previously saved (a good filename extension is .blk)
  5. To examine the current grid
        Toggle on, Mesh, then Select Yes to pop-up
        Toggle on, Project Faces, then Select Yes to pop-up
  6. Select Meshing (you may want to turn off the mesh for the next steps)
  7. Select Edge Params
  8. Select an edge to modify (left click on edge)
  9. Adjust the number of vertices (Num points)
  10. Toggle on, Copy to parallel edges
  11. Toggle on, All
  12. Select Apply
  13. To vary the mesh in other locations, select "Select new edge" and repeat steps 8, 9 and 12
  14. After all edges have been modified, select Done on the Edge meshing parameters pop-up
  15. Select Compute
  16. Toggle on Mesh and inspect grid, correct if necessary
  17. Perform a grid quality check with Quality check
  18. When satisfied with grid, exit Hexa-Interactive as follows so that new grid is available:
    1. toggle File
    2. click Save blocking (convention is to use .blk extension)
    3. click Multiblock
    4. choose Volume
    5. click Quit
    6. select Yes to Really quit
    7. select Yes to Load the new mesh Multiblock
    8. select Replace to next pop up
  19.  Toggle Output to output a new itape17:
  20. Assuming a boundary condition file has been read in, select KIVA-3(V) input
  21. Select All domains, then Done
  22. Toggle on KIVA-3V for kiva3v output
  23. Select Done
  24. The default itape17 file name is kiva3.tape17.  If your work was done on a PC and you intend to use the grid on a UNIX platform, then it is recommended that you open a UNIX window and issue the
    to_unix kiva3.tape17 itape17
    command, or equivalent so that the itape17 can be used on UNIX (note that the itape17 will be read properly on a PC too).
  25. Quit icem-cfd by toggling File, selecting Quit, then Yes to really quit.

What are appropriate boundary conditions for kiva3v sector grids?

This example is for a sector mesh with a square bowl and also includes the piston-liner crevice.

Click for ICEM-CFD boundary condition assignments that were used.

Click on any of the following to view flag values on the mesh surfaces:
bcb    bcf    bcl    f    fv    idface    idreg

If ICEM-CFD IJK orientation is not appropriate for kiva3v, how can it be fixed?

Courtesy of Christian Nienhueser

You can change the orientation of the blocks in Hexa > meshing >
ijk->kij (display the directions in the display window under blocks >
opts > ijk). More convenient is it to use the mesh editor once you wrote
the multiblock files in Hexa: MED > edit mesh > edit blocks >
orientation (display the directions in the display window under domains
> opts < show ijk).

How can I change the squish height of an existing mesh?

Courtesy of Kevin Dewey

You can simply move the geometry on the head and any curves near the head that are used to retain shape, or near head grid resolution up or down by the desired amount (ex: move curves up 4.129 cm).  Use "Geometry > Copy/Move" and select the entities you wish to move.  Select "Move" (default) and Translate, typing in the vector (ex: to increase the squish up by 4.129 (cm), enter 0 0 4.129) in the field and Accept.  This will create a gap in the periodic and liner faces.  It would probably be easiest to delete the existing surfaces and create new ones using the new curve positions.
 
In the blocking, you can use index control to turn off the the blocks beneath the head, or beneath the fine resolution region near the head (ex: K:5-6 for a particular case).  Then, you can move the visible blocks by going to "Topology > Transform, and very much similar to the copy/move panel in Geometry, type in the same  translation vector.  Then toward the bottom select "Only visible index range" and Apply.
 
You should not need to re-associate the edges.  The curves names won't change if you simply move  them in the geometry menu.  If you delete and recreate the curves, then you will have to re-associated edges.  For surfaces, it doesn't matter if they're recreated.

Can an itape17 be used in ICEM-CFD?

Courtesy of Kevin Dewey

Kind of.  There is a converter that converts an itape17 to domain files, which can be read into ICEM-CFD.   If you are at the ERC, ask Randy for the executable  for either a PC, or an SGI.
Usage: convert_itape17 [itape17] [icem domain file name]

Note:  The converter does not work with 4* format for repetitive fields.  Therefore, if the itape17 contains 4*0.0 to represent, replace it with 0.0 0.0 0.0 0.0, or as appropriate.

Is there any difference between piston/liner crevice representation in ICEM-CFD grids and those made with k3prep?

Not necessarily.  It is more a matter of how the grid builder chooses to make the grid.  Users of k3prep tend to assign the liner part of the crevice as a solid surface, where some users of ICEM-CFD assign this part of the liner to be moving.

What is a technique for getting nice curves on sharp edges?

Courtesy of Kevin Dewey

I suggest running "Geometry > Curve > Create > Build topology" to get the necessary curves.  These additional curves will add a constraint for tetra; forcing it to place nodes and edges on the curve to capture the feature.

If ICEM-CFD diagnostics tell me there are Multiple Edges, is that OK?

Courtesy of Kevin Dewey

Multiple edges may be legitimate.  These are edges that share more than 2 triangles so you would expect them at t-junctions, where the id and od of the head meet the liner would be t-junctions for which you would expect multiple edge elements. 

What do non-manifold elements indicate?

Courtesy of Kevin Dewey

Non-manifold vertices typically indicate elements that jump from one surface to another forming tent like structures.  Select "Help > Mesh editor > Edit mesh > Unstructured mesh options > Diagnostics > Check mesh > Possible problems" and scroll down to get a better description of non-manifold vertices.  [ Comments to a specific problem:  You have a few of these on the thin annular surface towards the top of the liner.  Once build topology is done, the surfaces will automatically be segmented which will allow you to prescribe a smaller element size on this surface (Geometry > Surface > Entity parameters)]. 

Are there guidelines for when to use automatic vs. manual fixes?

Courtesy of Kevin Dewey

For each diagnostic it is best to "Create subsets" instead of trying to automatically fix.  Auto fix for non-manifold and multiple edges will likely fail and auto fixing single edge problems will most likely make the mesh worse.  Only use the fix option for duplicate elements.  Once a subset is created, select it from the list at the bottom of the display menu.  Usually you want to display the adjoining elements to get a better picture of the problem area(s).  Select "Modify" beneath the subset list and "Add layer" in the pop-up menu.  Typically you want to add layers of surface elements only for which you can toggle "All F, Surfs" which means add only surface elements (tris) regardless of which family is active (turned on in the list at the top of the Display menu).  Then, you can do manual editing, such as merging nodes, splitting edges, deleting/creating elements, etc.  A good reference is the E-Tetra_Editing.ppt file within ftp://ftp.icemcfd.com/pub/training/4.2.2_Lectures.zip

[Comments to a specific problem:  I would use manual editing if you have only a few problem areas.  In your case, the geometry is so simple I would simply rerun tetra after you create the necessary curves and prescribe a smaller tetra size to the annular surface.  Actually, creating a hexa mesh would also be fairly easy.  Most structural solvers also prefer a hexa dominant mesh as well.]

Should spaces be avoided in directories and file names?

Courtesy of Kevin Dewey

Yes.

Do you have suggestions for creating an icem-cfd grid from an existing itape17?

Courtesy of Kevin Dewey

After reading in the mesh, you'll want to convert this to a blocking in Hexa.  If using the old gui (4.3 or older), you'll first have to create a tetin (geometry) file.  If you have the original geometry (iges, UG, etc.), import it into ICEM (File > Import geo).  If not, you can convert the mesh (mesh domain file) to faceted geometry (Geometry > Utilities > Transfer mesh -> facets).  Then go to "Meshing > Hexa > Interactive" save the tetin file  and start off with new blocking.  Then select "File > Load Mesh > Unstructured" and select the converted ICEM mesh.  You should wind up with a block topology that represents the imported mesh.  Then, typically you must associate edges to curves, move vertices, set node distrubtions, compute the mesh, etc...  basic Hexa procedures (similar to those shown in the ICEM tutorials)
 
Perhaps you might want to learn how to rebuild the mesh in ICEM.  Although more complicated than your sector model, it shouldn't be too difficult to create a mesh from scratch.  The nice thing about ICEM is that you can save the block topology and use it as a template for similar geometries.  It's also easy to dynamically update the node distributions and refinement and quickly recompute the mesh.

What must be done on-axis for sector grids in icem-cfd?

Courtesy of Jim Wiedenhoefer

You have to collapse the axis grid face.  It's an option in the mesh generator.

How can I bring up the old icem-cfd interface in version 5?

Page courtesy of Simon Pereira of ICEM-CFD

After installing ICEM CFD on Windows, you should have a shortcut, probably even one on the desk top.  Right Click on this ICON and select Properties from the pull down.  The Properties window will apear.  Look under the Shortcut Tab for the target path, you will see that it points to the icemcfd.bat file.  You need to run this file with the “-4” option.  Add a “ -4” to the end of the target line out side of the “quotation marks”.  See my below picture.  Then apply this change.  Next time the ICON is used, the old GUI will be summoned.

I should point out that the old GUI will not be available after the next release.  The new GUI has many new features that make it better and easier to use and learn.  If you want to get new training material, contact Mark.Malone@ANSYS.com.

Is there a way to assign different node counts to parallel edges?

Page courtesy of  Marlow Springer

The Hexa mesher is a block-structured mesher.  Thus, all parallel edges will automatically have the same node counts on them by default - due to the structured nature of the mesher.  In your case - you have a block in the VORFN volume family that creates the connection across the void space.  This arose from the process you followed to create the original blocking structure.

There is an easy way to break the connection.  Make sure all of your Volume Families of interest are active in the list (looks like you only have desired blocks in BOWL and SQUISH).  And hit Reset from the Index Control panel so everything is displayed.  Blocking > Delete Blocks > Blanked will permanently delete any blocks not displayed and re-create the VORFN region in an O-Grid fashion - thus breaking any connections across void spaces.  Now you can set the node counts as you specified.

What is needed to create surfaces in hexa?

Page courtesy of  Marlow Springer

To create surfaces you need sets of bounding curves to describe the surface boundaries.  Surfaces from 2 to 4 curves works best.  If more than 4 curves are used, it will try to build a trimmed/bounded plane.  So I would suggest building sets of surfaces bounded by 4 curves to build those remaining surfaces.

Options that you might need: Creating Curves , Modifying Curves (segmenting, merging), Creating Surfaces

Why does icem-cfd report different distances when using local coordiante systems?

Page courtesy of Matt Middleton

Q: I created a local coordinate system in the mesh editor of icem-cfd, version 4.2 on my PC.  Although the system looks fine, when I check the distance between two points, first in the global system, then in the local system, I get different distances.  I could not find an explanation for the Global and Local text boxes that are at the bottom of the Coordinate System pop-up window, so I left them blank.
A:  It's a known bug that's been fixed in our latest version. The workaround for your version is easy, though. After creating your local coordinate system, save your tetin, close it, and reload it. This problem only happened when you use prescribed points to create your local coordinate system or you specified vectors greater than one in length.