- 1 Background
- 2 Technical Objectives
- 3 Build Directions
- 4 Running the CoProcessing Script Generator
- 5 Creating the Adaptor
This work is supported under U.S. Army Research topic A07-010 proposal number A2-3295. The name of the project is CFD Co-Processing for Unsteady Visualization, Phase II. Several factors are driving the growth of CFD simulations. Computational power of computer clusters is growing while the price of individual computers is decreasing. Distributed computing techniques allow hundreds or even thousands of computer nodes to participate in a single simulation. The benefit of this computational power is that simulations are getting more accurate and useful for predicting complex phenomena. The downside to this growth in computational power is that enormous amounts of data need to be saved and analyzed to determine the results of the simulation. The ability to generate data has outpaced our ability to save and analyze the data. This bottle neck is throttling our ability to benefit from our improved computing resources. Simulations save their states only very infrequently to minimize storage requirements. This coarse temporal sampling makes it difficult to notice some complex fluid behavior.
Research and development to address this problem has focused on various solutions including data management, data reduction and compression, saliency analysis and feature extraction. However, there are very few solutions that bring these together and introduce them in the work-flow of the researcher. Furthermore, most of these solutions focus on deploying the post-processing tools on systems that do not scale as well as the ones the simulation codes run on. As mesh size, temporal resolution, problem complexity and parameter ranges grow, the analysis and visualization world has to adapt. The visualization tool developers can no longer assume that post-processing is a serial task that happens after the simulation on a dedicated graphics workstation. Rather, the processing of the data has to be tightly integrated with the simulation in order to scale with it. This will require rethinking of many visualization algorithms, development of new ones and also creation of the next generation analysis tools that share characteristics with simulation codes and can be deployed on the same supercomputers.
The main objective of the co-processing project is to integrate core data processing with the simulation to enable scalable data analysis. We will achieve this goal by building an end-to-end co-processing system.
- Develop an Extensible and Flexible Co-Processing Library. The co-processing library developed as part of the project has to be flexible enough to be embedded in various simulation codes with relative ease. This flexibility is critical, as a library that requires a lot of effort to embed cannot be successfully deployed in a large number of simulations. The co-processing library has to be easily extensible so that users can easily deploy new analysis and visualization techniques to existing co-processing installations.
- Develop Configuration Tools for Co-Processing Configuration. Based on conversations we had with our collaborators, we concluded that it is important for the users to be able to configure the co-processor using graphical user interfaces that are part of their daily work-flow. Therefore, we will develop a
graphical user interface to setup the co-processing pipelines.
Note that all of this must be done for large data. The co-processing library will almost always be run on a distributed system. For the largest simulation, the visualization of extracts may also require a distributed system (i.e. a visualization cluster).
The two components for doing coprocessing are a client-side plugin and a server side library. It is recommended that they be compiled separately but from the same ParaView source revision. This is because currently the server side library uses python which due to the wrapping will try to bring in all of the paraview libraries which it could potentially need. This means that it will try to bring in objects that require a terminal window to display to which may cause problems on clusters and supercomputers.
ParaView Coprocessing Script Generator Plugin
The plugin for generating python scripts for coprocessing is a client-side plugin. The CMake option to turn on the script generator plugin is PARAVIEW_BUILD_PLUGIN_CoProcessingScriptGenerator. Note that since this is a client-side plugin that the PARAVIEW_BUILT_QT_GUI option must be on.
The directions for building the coprocessing library can be a bit more complex. We assume that it will be built on a cluster or supercomputer. Complexities may arise from having to build mesa, use off-screen rendering, build static libraries, and/or cross-compiling. We won't go into those details here though but refer interested people to the ParaView and VTK wikis.
The addition flags that should be turned on for coprocessing include:
- BUILD_SHARED_LIBS Should normally be set to ON unless you're compiling on a machine that doesn't support shared libs (e.g. IBM BG/l).
- PARAVIEW_ENABLE_PYTHON Set to ON in order to use the scripts created from the coprocessing plugin.
- PARAVIEW_USE_MPI Set the ParaView server to use MPI to run in parallel. Also check that the proper version of MPI is getting used.
- CMAKE_BUILD_TYPE Should be set to Release in order to optimize the ParaView code.
- PARAVIEW_ENABLE_COPROCESSING The CMake option to build the coprocessing libraries.
- BUILD_COPROCESSING_ADAPTORS The CMake option to turn on code that may be useful for creating the simulation code adaptor.
- BUILD_FORTRAN_COPROCESSING_ADAPTORS The CMake option to turn on code that may be useful for creating an adaptor for a simulation code written in Fortran or C.
- PYTHON_ENABLE_MODULE_vtkCoProcessorPython On by default.
- BUILD_PYTHON_COPROCESSING_ADAPTOR Experimental code.
To test that the coprocessing library is working on your system use the command ctest -R CoProcessing. The CoProcessingTestPythonScript test does an actual coprocessing run and the CoProcessingPythonScriptGridPlot and CoProcessingPythonScriptPressurePlot test verify the output is correct. Note that by using ctest -V -R CoProcessingTestPythonScript you can see the verbose output if the test. Looking at the code for this test is a useful beginning point for learning to use the coprocessing library.
If you are using Mesa, the following options should be used:
- VTK_OPENGL_HAS_OSMESA Set to ON.
- OSMESA_INCLUDE_DIR, OPENGL_xmesa_INCLUDE_DIR and OPENGL_INCLUDE_DIR Make sure this is not set to the OpenGL version of the header files.
- OSMESA_LIBRARY, OPENGL_gl_LIBRARY and OPENGL_glu_LIBRARY Set these to the proper libraries.
- VTK_USE_OFFSCREEN Set to ON
Running the CoProcessing Script Generator
After starting the ParaView client, go to Tools->Manage Plugins, highlight CoProcessingPlugin and click Load Selected. Alternatively, if you expect to be using this plugin often you can tell ParaView to automatically load the plugin by clicking to the left of CoProcessingPlugin to expand the list and choose the Auto Load option. This will add a CoProcessing and Writers menu to the GUI.
Once the plugin is loaded, load a simulation result into ParaView that is similar to the run you wish to do coprocessing with. Normally the result will be for a discretization of the same geometry and contain the same field variables (or at least all of the field variables you wish to examine) as the simulation grid that coprocessing will be performed on. The only difference between these two grids will be that the grid used for the coprocessing run will be at a much higher resolution. In the picture below, a pipeline is shown for a result from a PHASTA (A CFD code led by Ken Jansen at the University of Colorado) simulation of incompressible flow through an aortic aneurysm. The simulation results include the velocity and pressure fields and was done on a grid with 235,282 cells and 45,175 points. It is important to use the same names for the field arrays as will be used in the grids the coprocessing library will be working with. The filters specify which fields to use by their name and problems will occur if the filters cannot find the correct array. The pipeline computes the vorticity, takes 20 slices through the domain, and extracts the surface of the grid.
Once the pipeline is set up, you must add in the writers to use for the filters that you want results from. Do this by selecting the appropriate writer to output the results from each desired filter. In this example we create a ParallelPolyDataWriter for the Slice filter and the ExtractSurface filter. For the writer for the Slice filter we set the name of the file to be slice_%t.pvtp where %t will get replaced with the time step each time it is output. We also set the write frequency to be every fifth time step. The picture below shows this.
Similarly, we do the same for the writer for the ExtractSurface filter but we want to use a different file name and we can set a different write frequency if desired.
Note that when we hit enter we get the error message Cannot show the data in the current view although the view reported that it can show the data. This message can be ignored and is already entered as a bug to fix in ParaView.
The final step is to go through the CoProcessing->Export State wizard to associate the grid with a name that they python script uses and specify a file name for the script. The steps are:
1. Export Co-Processing State Click Next to proceed.
2. Select Simulation Inputs Choose which grids to use by highlighting the grid and clicking Add, then click Next.
3. Name Simulation Inputs Click in the boxes under Simulation Name and change the name to what you have named the grid in your adaptor. Our convention is to use "input" for simulations with a single grid or multiblock data set.
4. Configuration We usually want the full data and not just a picture of the results so for this we leave "Output rendering components i.e. views" unchecked and just hit Finish.
If we do want to output images in addition to any writers we may have specified, check "Output rendering components i.e. views" and fill in the proper information. Note that the image type is specified based on the file name extension and that %t will be replaced by the actual time step in the output file name. Additionally, if there are multiple views then %v will be replaced by the view index in the ouptput file name.
5. Save Server State: Specify the file name the script is to be saved as.
The resulting python script should look something like:
try: paraview.simple except: from paraview.simple import * cp_writers =  def RequestDataDescription(datadescription): "Callback to populate the request for current timestep" timestep = datadescription.GetTimeStep() if (timestep % 5 == 0) or (timestep % 200 == 0) : datadescription.GetInputDescriptionByName('input').AllFieldsOn() datadescription.GetInputDescriptionByName('input').GenerateMeshOn() def DoCoProcessing(datadescription): "Callback to do co-processing for current timestep" global cp_writers cp_writers =  timestep = datadescription.GetTimeStep() grid5_0_vtu = CreateProducer( datadescription, "input" ) GradientOfUnstructuredDataSet1 = GradientOfUnstructuredDataSet( guiName="GradientOfUnstructuredDataSet1", ScalarArray=['POINTS', 'velocity'], ResultArray Name='Vorticity', ComputeVorticity=1, FasterApproximation=0 ) Slice2 = Slice( guiName="Slice2", SliceOffsetValues=[-10.23284210526316, -8.8684631578947375, -7.5040842105263152, -6.1397052631578966, -4.77532631578947 43, -3.4109473684210529, -2.0465684210526316, -0.68218947368421201, 0.68218947368420935, 2.0465684210526316, 3.4109473684210521, 4.7753263157894743, 6.139705 263157893, 7.5040842105263152, 8.8684631578947375, 10.23284210526316, 11.597221052631578, 12.961600000000001], SliceType="Plane" ) SetActiveSource(GradientOfUnstructuredDataSet1) ExtractSurface1 = ExtractSurface( guiName="ExtractSurface1", PieceInvariant=1 ) SetActiveSource(Slice2) ParallelPolyDataWriter3 = CreateWriter( XMLPPolyDataWriter, "slice_%t.pvtp", 5 ) SetActiveSource(ExtractSurface1) ParallelPolyDataWriter2 = CreateWriter( XMLPPolyDataWriter, "surface_%t.pvtp", 200 ) Slice2.SliceType.Origin = [-2.8049160242080688, 2.1192346811294556, 1.7417440414428711] Slice2.SliceType.Offset = 0.0 Slice2.SliceType.Normal = [0.0, 0.0, 1.0] for writer in cp_writers: if timestep % writer.cpFrequency == 0: writer.FileName = writer.cpFileName.replace("%t", str(timestep)) writer.UpdatePipeline() def CreateProducer(datadescription, gridname): "Creates a producer proxy for the grid" if not datadescription.GetInputDescriptionByName(gridname): raise RuntimeError, "Simulation input name '%s' does not exist" % gridname grid = datadescription.GetInputDescriptionByName(gridname).GetGrid() producer = TrivialProducer() producer.GetClientSideObject().SetOutput(grid) producer.UpdatePipeline() return producer def CreateWriter(proxy_ctor, filename, freq): global cp_writers writer = proxy_ctor() writer.FileName = filename writer.add_attribute("cpFrequency", freq) writer.add_attribute("cpFileName", filename) cp_writers.append(writer) return writer
Creating the Adaptor
The largest amount of work in getting coprocessing working with a simulation code is usually creating the adaptor that can pass a VTK data set or composite data set with fields specified over it. A simple view of the program control is
By doing it like this, there is minimal modification to the simulation code (only calls to the adaptor like Initialize, Finalize, and CoProcess). The adaptor deals with the coprocessing library as well as creating VTK data structures from the simulation code as needed. The general flow for the simulation code and where it calls the adaptor would look like:
initialize coprocessor for i in number of time steps compute simulation information at time step i call coprocessing library coprocessing library determines if any coprocessing needs to be performed at time step i finalize coprocessor
The interactions between the adaptor and ParaView are mostly done through the vtkCPProcessor class. Documentation for this and the other classes in the coprocessing library are in the ParaView online documentation as well as grouped in a module. Details on the specific steps are provided below.
Initialize the CoProcessor
To initialize the coprocessor, a vtkCPProcessor object must be created. This object should not be deleted until the finalization step. After creating a vtkCPProcessor object, you must call vtkCPProcessor::Initialize() to initialize the coprocessing library. The next step is to create vtkCPPipeline objects. These objects are used to represent the VTK pipelines that will be used to generate the output data. Most users will probably only use the vtkCPPythonScriptPipeline class that derives from vtkCPPipeline since that pipeline is the one that is used with the python scripts generated from the coprocessing plugin. vtkCPPythonScriptPipeline::Initialize() takes in the python script name with the full path and sets up the ParaView python interpretor.
Call the CoProcessor to Execute the Desired Filters
Most users will have a single call to the adaptor at the end of each simulation time step. This will pass in the simulation data structures to create the VTK data structures from. The created VTK data structures will be some type object that derives from vtkDataObject. First though we want to check if we actually need to do any coprocessing during this call. The simulation code will not know this information. Because of this, the simulation code should call the adaptor every time step. The adaptor gets the information about what data is needed for executing the vtkCPPipelines for each call. This is done in vtkCPProcessor::RequestDataDescription() by going through all of the vtkCPPipeline objects and querying them for what is needed. vtkCPProcessor::RequestDataDescription() takes in a vtkCPDataDescription object that contains information about the current simulation time and time step. The method returns 0 if no coprocessing information needs to be computed during the call and 1 otherwise. If no coprocessing needs to be performed then the adaptor should return control back to the simulation code.
If coprocessing is requested then the adaptor needs to make sure that the VTK grids and fields are up to date. Upon return from vtkCPProcessor::RequestDataDescription(), the vtkCPDataDescription object will have information on what is needed by the pipelines in order to successfully execute them during this call to the adaptor. This information is stored for each coprocessing input (the data objects that are given identifier names in the plugin) and accessed through the vtkCPDataDescription as vtkCPInputDataDescription objects. The vtkCPInputDataDescription objects specify whether or not they require a grid and if so which fields they require. These objects are also used to pass the VTK data objects created in the adaptor to the pipeline by using the vtkCPInputDataDescription::SetGrid() method. The final step in this call to the adaptor is then to perform the actual coprocessing by calling the vtkCPProcessor::CoProcess() method.
Finalize the CoProcessor
Finalization entails calling vtkCPProcessor::Finalize() and cleaning up any remaining VTK objects by calling Delete();
While initially there may seem to be a significant hurdle to overcome in order to implement the adaptor for coprocessing, the user only needs to know enough information to create the VTK data objects from their own simulation data structures. The adaptor can be made computationally efficient by taking advantage of intimate knowledge of the simulation code and knowing that VTK filters will not modify input data. Examples include:
- Only creating the VTK grid in the first call to the adaptor if the grid is not changing topologically or geometrically.
- Using the SetArray() method to build vtkDataArray objects that use existing memory used by the simulation code instead of allocating and copying existing memory.
Finally, we suggest looking at the code in ParaView3/CoProcessing/CoProcessor/Testing/Cxx/PythonScriptCoProcessingExample.cxx to see how the entire coprocessing flow works.