Solution classes
Last update: 20.02.2025Solution
class compolyx.Solution(obj, parent=None)
Class to compute postprocessings of a finite element solution.
Access:
>>> import compolyx
>>> db = compolyx.DB()
>>> model = db.models['class40.1']
>>> sol = db.models['class40.1'].add_solution(name='class40.1', path='class40.rst', format='ansys:rst')
property ID
Id to be displayed in Envelope solution.
property active
Activate or deactivate solution.
clear()
Clear all result data.
clear_element_results()
Resets the postprocessing results for each layered element.
clear_failure_criteria_results()
Resets the failure criteria results for each layered element.
property enabled
Whether this object is currently enabled or not. Mainly defined through the current application mode pre or post.
export_results_to_csv(definition=None, entities=[], file_path=None, solution_set=-1, solids=False, spot='all')
Exports the shell results of the selected entities to a csv file.
- Parameters:
- definitions: Selected definition - CombinedFailure Criteria object or as string ‘deformations’, ‘strains’, or ‘stresses’.
- entities: Defines the selection for the export. Can be a list of ElementSets, AnalysisPlies, or SolidModels.
- file_path: File name.
- solution_set: Solution Set for which data is requested.
- solids: Boolean whether to take the results of the solid elements or not. Default is False (results of shells).
- spots: Layer positions for which the results are exported. Allowed are ‘bot’, ‘mid’, ‘top’, ‘bot/top’, and ‘all’.
Export results of solid models: Choose the element set which is selected in the extrusion settings.
- Usage:
>>> model = db.active_model >>> model.solutions['Solution.1'].export_results_to_csv( definition='stresses', entities=[model.element_sets['BULKHEAD_ALL']], file_path=r'C: mp\stresses.csv', solution_set=1, solids=False, spot='bot-top')
property ext_id
Id of corresponding Solution in external solution (ComponentID).
property format
File format string. Choose one of ‘abaqus:inp’,’ansys:cdb’, or ‘nastran:f06’.
property has_element_temperatures
Boolean flag if element nodal temperatures are read from the rst file.
property has_progressive_damage
Boolean flag if progressive_damage data are read from the rst file.
load()
Load result data from file.
property load_factor
Optional load factor within substep of non-linear solution where the nodal solution should be taken from. Only valid for ‘nastran:f06’ format. Becomes (False,0) if not defined.
property path
Path to the data file.
property path2
Path to the data file.
property plots
Container with PostProcessing Plots.
query(definition, options={'eval_ins': False}, position='centroid', selection='all', entity=None, entities=None, spot=None, component=None, rosette=None, simulate=False, solution_set=-1)
Query results from the solution.
- Parameters:
- definition: The postprocess definition defines what results are evaluated. Can be given as CombinedFailureCriteria object or as string such as ‘strains’, ‘stresses’, ‘laminate_forces’, ‘deformations’, ‘temperatures’, or ‘progressive_damage’.
- options: Dict with the additional options used to fully configure the definition.
- stresses: options = {“eval_ins”:True} to enable the interlaminar normal stress evaluation for shells.
- position: Position where data is queried:
- nodal, centroid, element_nodal, integration_point, or element_results.
- selection: The selection set determines the selected nodes and elements. Can be given as string ‘sel0’ - ‘sel5’ or ‘all’, or can be given as ObjectSelection object such as model.selection or scene.active_set.
- entity: Entity for which results are evaluated. Currently supported: Analysis ply or analysis ply vertex.
- entities: If a list of entities is given, the query will also compute and return a list of results, with one array for each entity.
- spot: Used to identify bot, mid or top when querying layered shells.
- component: Components to query. Valid components for
- DEFORMATION
- x, y, z, usum, rotx, roty, rotz -> (nx1).
- all -> (nx6), translations, rotations -> (nx3).
- STRAIN
- e1, e2, e3, e12, e23, e13, eI, eII, eII, von_mises -> (nx1).
- all -> (nx6), principals -> (nx3).
- STRESS
- s1, s2, s3, s12, s23, s13, sI, sII, sII -> (nx1).
- all -> (nx6), principals -> (nx3).
- FAILURE CRITERIA
- irf (Inverse reserve factor), rf (Reserve factor), mos (Margin of safety) -> (nx1).
- fm (Failure mode) ->(n x string(size<=4))
- li (Layer index) ->(n x 1) (Only available for element queries where no entity is given.).
- LAMINATE FORCES
- all -> (nx8).
- PROGRESSIVE DAMAGE
- status (damage status), ft, fc (fiber tensile/compressive) ->(nx1).
- mt, mc (matrix tensile/compressive), s (shear) ->(nx1).
- sed (energy dissipated per unit volume), sedv (energy per unit volume due to viscous damping) ->(nx1).
- DEFORMATION
- rosette: If a rosette is given, the results are evaluated with respect to this coordinate system (not recommended for non-linear results).
- simulate: Whether the query is only simulated to test if it will return data. If this flag is set the query(…) function will only return 0 or 1.
- solution_set: Identifier of the queried solution. -1 identifies the last available Set.
- Usage:
>>> solution.query(definition='laminate_forces',position='centroid',selection='sel0',component='all',rosette=model.rosetttes['Rosette.1'],solution_set=-1) >>> solution.query(definition=model.defintions['FailureCriteria'], position='centroid', selection='sel0', component='irf',solution_set=-1) >>> solution.query(definition='stresses', position='element_results', selection='sel0', component='s3',solution_set=-1)
property read_stresses_strains
True if the stresses and strains are to be read from rst file. Only valid for ‘ansys:rst’ format.
property recompute_iss_of_solids
Use laminate-based computation method to recalculate the interlaminar shear stress distribution.
property renumbering_mapping_paths
Path of the assembly renumbering files.
serialize()
Serialize to Python string.
property set
Result set to be read. Only valid for ‘ansys:rst’ format.
property solution_dict
The time or frequency dictionary used in the solution plots GUI.
property subcase
Optional subcase to read. Only valid for ‘nastran:f06’ format. Becomes (False,0) if not defined.
property time_or_frequency
The time or frequency associated with the active set.
property use_felyx_to_compute_pp_results
True if the stresses and strains are to be computed by felyx. If the stresses and strains are read from .rst file, nothing is computed.
property use_solid_results
Allows to visualize the postprocessing results of layered solid models on the ‘Layered Solid Reference Surface’.
EnvelopeSolution
class compolyx.EnvelopeSolution(graph, obj, parent=None)
add_solution_set(solution, sset=-1)
Add solution set to solution sets of Envelope Solution.
- Parameters:
- solution: Solution object.
- sset: Solution set (default: -1).
clear_solution_sets()
Clear Solution Sets of Envelope Solution.
property enabled
Whether this object is currently enabled or not. Mainly defined through the current application mode pre or post.
remove_solution_set(solution, sset=-1)
Remove solution set from solution sets of Envelope Solution.
- Parameters:
- solution: Solution object.
- sset: Solution set (default: -1).