ccxInpWriter.py

# ***************************************************************************
# *                                                                         *
# *   Copyright (c) 2015 - Przemo Firszt <przemo@firszt.eu>                 *
# *   Copyright (c) 2015 - Bernd Hahnebach <bernd@bimstatik.org>            *
# *                                                                         *
# *   This program is free software; you can redistribute it and/or modify  *
# *   it under the terms of the GNU Lesser General Public License (LGPL)    *
# *   as published by the Free Software Foundation; either version 2 of     *
# *   the License, or (at your option) any later version.                   *
# *   for detail see the LICENCE text file.                                 *
# *                                                                         *
# *   This program is distributed in the hope that it will be useful,       *
# *   but WITHOUT ANY WARRANTY; without even the implied warranty of        *
# *   MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the         *
# *   GNU Library General Public License for more details.                  *
# *                                                                         *
# *   You should have received a copy of the GNU Library General Public     *
# *   License along with this program; if not, write to the Free Software   *
# *   Foundation, Inc., 59 Temple Place, Suite 330, Boston, MA  02111-1307  *
# *   USA                                                                   *
# *                                                                         *
# ***************************************************************************


import FreeCAD
import os
import sys
import time


__title__ = "ccxInpWriter"
__author__ = "Przemo Firszt, Bernd Hahnebach"
__url__ = "http://www.freecadweb.org"


class inp_writer:
    def __init__(self, analysis_obj, mesh_obj, mat_obj,
                 fixed_obj,
                 force_obj, pressure_obj,
                 beamsection_obj, shellthickness_obj,
                 analysis_type=None, eigenmode_parameters=None,
                 dir_name=None):
        self.dir_name = dir_name
        self.analysis = analysis_obj
        self.mesh_object = mesh_obj
        self.material_objects = mat_obj
        self.fixed_objects = fixed_obj
        self.force_objects = force_obj
        self.pressure_objects = pressure_obj
        if eigenmode_parameters:
            self.no_of_eigenfrequencies = eigenmode_parameters[0]
            self.eigenfrequeny_range_low = eigenmode_parameters[1]
            self.eigenfrequeny_range_high = eigenmode_parameters[2]
        self.analysis_type = analysis_type
        self.beamsection_objects = beamsection_obj
        self.shellthickness_objects = shellthickness_obj
        if not dir_name:
            self.dir_name = FreeCAD.ActiveDocument.TransientDir.replace('\\', '/') + '/FemAnl_' + analysis_obj.Uid[-4:]
        if not os.path.isdir(self.dir_name):
            os.mkdir(self.dir_name)
        self.base_name = self.mesh_object.Name
        self.file_name = self.dir_name + '/' + self.base_name + '.inp'
        self.fc_ver = FreeCAD.Version()
        self.ccx_eall = 'Eall'
        self.ccx_elsets = []

    def write_calculix_input_file(self):
        self.mesh_object.FemMesh.writeABAQUS(self.file_name)

        # reopen file with "append" and add the analysis definition
        inpfile = open(self.file_name, 'a')
        inpfile.write('\n\n')
        self.write_element_sets_material_and_femelement_type(inpfile)
        self.write_node_sets_constraints_fixed(inpfile)
        self.write_node_sets_constraints_force(inpfile)
        self.write_materials(inpfile)
        self.write_femelementsets(inpfile)
        self.write_step_begin(inpfile)
        self.write_constraints_fixed(inpfile)
        if self.analysis_type is None or self.analysis_type == "static":
            self.write_constraints_force(inpfile)
            self.write_constraints_pressure(inpfile)
        elif self.analysis_type == "frequency":
            self.write_frequency(inpfile)
        self.write_outputs_types(inpfile)
        self.write_step_end(inpfile)
        self.write_footer(inpfile)
        inpfile.close()
        return self.file_name

    def write_element_sets_material_and_femelement_type(self, f):
        if len(self.material_objects) == 1:
            if self.beamsection_objects and len(self.beamsection_objects) == 1:          # single mat, single beam
                self.get_ccx_elsets_single_mat_single_beam()
            elif self.beamsection_objects and len(self.beamsection_objects) > 1:         # single mat, multiple beams
                self.get_ccx_elsets_single_mat_multiple_beam()
            elif self.shellthickness_objects and len(self.shellthickness_objects) == 1:  # single mat, single shell
                self.get_ccx_elsets_single_mat_single_shell()
            elif self.shellthickness_objects and len(self.shellthickness_objects) > 1:   # single mat, multiple shells
                self.get_ccx_elsets_single_mat_multiple_shell()
            else:                                                                        # single mat, solid
                self.get_ccx_elsets_single_mat_solid()
        else:
            if self.beamsection_objects and len(self.beamsection_objects) == 1:         # multiple mats, single beam
                self.get_ccx_elsets_multiple_mat_single_beam()
            elif self.beamsection_objects and len(self.beamsection_objects) > 1:        # multiple mats, multiple beams
                self.get_ccx_elsets_multiple_mat_multiple_beam()
            if self.shellthickness_objects and len(self.shellthickness_objects) == 1:   # multiple mats, single shell
                self.get_ccx_elsets_multiple_mat_single_shell()
            elif self.shellthickness_objects and len(self.shellthickness_objects) > 1:  # multiple mats, multiple shells
                self.get_ccx_elsets_multiple_mat_multiple_shell()
            else:                                                                       # multiple mats, solid
                self.get_ccx_elsets_multiple_mat_solid()
        f.write('\n***********************************************************\n')
        f.write('** Element sets for materials and FEM element type (solid, shell, beam)\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        for ccx_elset in self.ccx_elsets:
            # print(ccx_elset)
            f.write('*ELSET,ELSET=' + ccx_elset['ccx_elset_name'] + '\n')
            if ccx_elset['ccx_elset'] == self.ccx_eall:
                f.write(self.ccx_eall + '\n')
            else:
                for elid in ccx_elset['ccx_elset']:
                    f.write(str(elid) + ',\n')

    def write_node_sets_constraints_fixed(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Node set for fixed constraint\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        for fobj in self.fixed_objects:
            fix_obj = fobj['Object']
            f.write('*NSET,NSET=' + fix_obj.Name + '\n')
            for o, elem in fix_obj.References:
                fo = o.Shape.getElement(elem)
                n = []
                if fo.ShapeType == 'Face':
                    n = self.mesh_object.FemMesh.getNodesByFace(fo)
                elif fo.ShapeType == 'Edge':
                    n = self.mesh_object.FemMesh.getNodesByEdge(fo)
                elif fo.ShapeType == 'Vertex':
                    n = self.mesh_object.FemMesh.getNodesByVertex(fo)
                for i in n:
                    f.write(str(i) + ',\n')

    def write_node_sets_constraints_force(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Node sets for loads\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        for fobj in self.force_objects:
            frc_obj = fobj['Object']
            f.write('*NSET,NSET=' + frc_obj.Name + '\n')
            NbrForceNodes = 0
            for o, elem in frc_obj.References:
                fo = o.Shape.getElement(elem)
                n = []
                if fo.ShapeType == 'Edge':
                    n = self.mesh_object.FemMesh.getNodesByEdge(fo)
                elif fo.ShapeType == 'Vertex':
                    n = self.mesh_object.FemMesh.getNodesByVertex(fo)
                for i in n:
                    f.write(str(i) + ',\n')
                    NbrForceNodes = NbrForceNodes + 1   # NodeSum of mesh-nodes of ALL reference shapes from force_object
            # calculate node load
            if NbrForceNodes != 0:
                fobj['NodeLoad'] = (frc_obj.Force) / NbrForceNodes
                #  FIXME for loads on edges the node count is used to distribute the load on the edges.
                #  In case of a not uniform fem mesh this could result in wrong force distribution
                #  and thus in wrong analysis results. see  def write_constraints_force()
                f.write('** concentrated load [N] distributed on all mesh nodes of the given shapes\n')
                f.write('** ' + str(frc_obj.Force) + ' N / ' + str(NbrForceNodes) + ' Nodes = ' + str(fobj['NodeLoad']) + ' N on each node\n')
            if frc_obj.Force == 0:
                print('  Warning --> Force = 0')

    def write_materials(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Materials\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        f.write('** Young\'s modulus unit is MPa = N/mm2\n')
        for m in self.material_objects:
            mat_obj = m['Object']
            # get material properties
            YM = FreeCAD.Units.Quantity(mat_obj.Material['YoungsModulus'])
            YM_in_MPa = YM.getValueAs('MPa')
            PR = float(mat_obj.Material['PoissonRatio'])
            mat_name = mat_obj.Material['Name'][:80]
            # write material properties
            f.write('*MATERIAL, NAME=' + mat_name + '\n')
            f.write('*ELASTIC \n')
            f.write('{}, \n'.format(YM_in_MPa))
            f.write('{0:.3f}\n'.format(PR))
            density = FreeCAD.Units.Quantity(mat_obj.Material['Density'])
            density_in_tone_per_mm3 = float(density.getValueAs('t/mm^3'))
            f.write('*DENSITY \n')
            f.write('{0:.3e}, \n'.format(density_in_tone_per_mm3))

    def write_femelementsets(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Sections\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        for ccx_elset in self.ccx_elsets:
            if 'beamsection_obj'in ccx_elset:  # beam mesh
                beamsec_obj = ccx_elset['beamsection_obj']
                elsetdef = 'ELSET=' + ccx_elset['ccx_elset_name'] + ', '
                material = 'MATERIAL=' + ccx_elset['ccx_mat_name']
                setion_def = '*BEAM SECTION, ' + elsetdef + material + ', SECTION=RECT\n'
                setion_geo = str(beamsec_obj.Height.getValueAs('mm')) + ', ' + str(beamsec_obj.Width.getValueAs('mm')) + '\n'
                f.write(setion_def)
                f.write(setion_geo)
            elif 'shellthickness_obj'in ccx_elset:  # shell mesh
                shellth_obj = ccx_elset['shellthickness_obj']
                elsetdef = 'ELSET=' + ccx_elset['ccx_elset_name'] + ', '
                material = 'MATERIAL=' + ccx_elset['ccx_mat_name']
                setion_def = '*SHELL SECTION, ' + elsetdef + material + '\n'
                setion_geo = str(shellth_obj.Thickness.getValueAs('mm')) + '\n'
                f.write(setion_def)
                f.write(setion_geo)
            else:  # solid mesh
                elsetdef = 'ELSET=' + ccx_elset['ccx_elset_name'] + ', '
                material = 'MATERIAL=' + ccx_elset['ccx_mat_name']
                setion_def = '*SOLID SECTION, ' + elsetdef + material + '\n'
                f.write(setion_def)

    def write_step_begin(self, f):
        f.write('\n***********************************************************\n')
        f.write('** One step is needed to calculate the mechanical analysis of FreeCAD\n')
        f.write('** loads are applied quasi-static, means without involving the time dimension\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        f.write('*STEP\n')
        f.write('*STATIC\n')

    def write_constraints_fixed(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Constaints\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        for fixed_object in self.fixed_objects:
            fix_obj_name = fixed_object['Object'].Name
            f.write('*BOUNDARY\n')
            f.write(fix_obj_name + ',1\n')
            f.write(fix_obj_name + ',2\n')
            f.write(fix_obj_name + ',3\n')
            if self.beamsection_objects or self.shellthickness_objects:
                f.write(fix_obj_name + ',4\n')
                f.write(fix_obj_name + ',5\n')
                f.write(fix_obj_name + ',6\n')
            f.write('\n')

    def write_constraints_force(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Node loads\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        if is_shell_mesh(self.mesh_object.FemMesh) or (is_solid_mesh(self.mesh_object.FemMesh) and has_no_face_data(self.mesh_object.FemMesh)):
            if not hasattr(self, 'fem_element_table'):
                self.fem_element_table = getFemElementTable(self.mesh_object.FemMesh)
        for fobj in self.force_objects:
            frc_obj = fobj['Object']
            if 'NodeLoad' in fobj:   # load on edges or vertieces
                node_load = fobj['NodeLoad']
                frc_obj_name = frc_obj.Name
                vec = frc_obj.DirectionVector
                f.write('*CLOAD\n')
                f.write('** force: ' + str(node_load) + ' N,  direction: ' + str(vec) + '\n')
                v1 = "{:.13E}".format(vec.x * node_load)
                v2 = "{:.13E}".format(vec.y * node_load)
                v3 = "{:.13E}".format(vec.z * node_load)
                f.write(frc_obj_name + ',1,' + v1 + '\n')
                f.write(frc_obj_name + ',2,' + v2 + '\n')
                f.write(frc_obj_name + ',3,' + v3 + '\n\n')

            # area load on faces
            sum_ref_face_area = 0
            sum_ref_face_node_area = 0
            sum_node_load = 0
            for o, elem in frc_obj.References:
                elem_o = o.Shape.getElement(elem)
                if elem_o.ShapeType == 'Face':
                    sum_ref_face_area += elem_o.Area
            if sum_ref_face_area != 0:
                force_per_sum_ref_face_area = frc_obj.Force / sum_ref_face_area

            for o, elem in frc_obj.References:
                elem_o = o.Shape.getElement(elem)
                if elem_o.ShapeType == 'Face':
                    ref_face = elem_o
                    f.write('** ' + frc_obj.Name + '\n')
                    f.write('*CLOAD\n')
                    f.write('** node loads on element face: ' + o.Name + '.' + elem + '\n')

                    face_table = {}  # { meshfaceID : ( nodeID, ... , nodeID ) }
                    if is_solid_mesh(self.mesh_object.FemMesh):
                        if has_no_face_data(self.mesh_object.FemMesh):
                            ref_face_volume_elements = self.mesh_object.FemMesh.getccxVolumesByFace(ref_face)  # list of tupels
                            ref_face_nodes = self.mesh_object.FemMesh.getNodesByFace(ref_face)
                            for ve in ref_face_volume_elements:
                                veID = ve[0]
                                ve_ref_face_nodes = []
                                for nodeID in self.fem_element_table[veID]:
                                    if nodeID in ref_face_nodes:
                                        ve_ref_face_nodes.append(nodeID)
                                face_table[veID] = ve_ref_face_nodes  # { volumeID : ( facenodeID, ... , facenodeID ) }
                        else:
                            volume_faces = self.mesh_object.FemMesh.getVolumesByFace(ref_face)   # (mv, mf)
                            for mv, mf in volume_faces:
                                face_table[mf] = self.mesh_object.FemMesh.getElementNodes(mf)
                    elif is_shell_mesh(self.mesh_object.FemMesh):
                        ref_face_nodes = self.mesh_object.FemMesh.getNodesByFace(ref_face)
                        ref_face_elements = getFemElementsByNodes(self.fem_element_table, ref_face_nodes)
                        for mf in ref_face_elements:
                            face_table[mf] = self.fem_element_table[mf]

                    # calulate the appropriate node_areas for every node of every mesh face (mf)
                    # G. Lakshmi Narasaiah, Finite Element Analysis, p206ff
                    # FIXME only gives exact results in case of a real triangle. If for S6 or C3D10 elements
                    # the midnodes are not on the line between the end nodes the area will not be a triangle
                    # see http://forum.freecadweb.org/viewtopic.php?f=18&t=10939&start=40#p91355  and ff

                    #  [ (nodeID,Area), ... , (nodeID,Area) ]  some nodes will have more than one entry
                    node_area_table = []
                    #  { nodeID : Area, ... , nodeID:Area }  AreaSum for each node, one entry for each node
                    node_sumarea_table = {}
                    mesh_face_area = 0
                    for mf in face_table:
                        if len(face_table[mf]) == 3:  # 3 node mesh face triangle
                            # corner_node_area = mesh_face_area / 3.0
                            #      P3
                            #      /\
                            #     /  \
                            #    /____\
                            #  P1      P2
                            P1 = self.mesh_object.FemMesh.Nodes[face_table[mf][0]]
                            P2 = self.mesh_object.FemMesh.Nodes[face_table[mf][1]]
                            P3 = self.mesh_object.FemMesh.Nodes[face_table[mf][2]]

                            mesh_face_area = getTriangleArea(P1, P2, P3)
                            corner_node_area = mesh_face_area / 3.0

                            node_area_table.append((face_table[mf][0], corner_node_area))
                            node_area_table.append((face_table[mf][1], corner_node_area))
                            node_area_table.append((face_table[mf][2], corner_node_area))

                        elif len(face_table[mf]) == 4:  # 4 node mesh face quad
                            FreeCAD.Console.PrintError('Face load on 4 node quad faces are not supported\n')

                        elif len(face_table[mf]) == 6:  # 6 node mesh face triangle
                            # corner_node_area = 0
                            # middle_node_area = mesh_face_area / 3.0
                            #         P3
                            #         /\
                            #        /t3\
                            #       /    \
                            #     P6------P5
                            #     / \ t4 / \
                            #    /t1 \  /t2 \
                            #   /_____\/_____\
                            # P1      P4      P2
                            P1 = self.mesh_object.FemMesh.Nodes[face_table[mf][0]]
                            P2 = self.mesh_object.FemMesh.Nodes[face_table[mf][1]]
                            P3 = self.mesh_object.FemMesh.Nodes[face_table[mf][2]]
                            P4 = self.mesh_object.FemMesh.Nodes[face_table[mf][3]]
                            P5 = self.mesh_object.FemMesh.Nodes[face_table[mf][4]]
                            P6 = self.mesh_object.FemMesh.Nodes[face_table[mf][5]]

                            mesh_face_t1_area = getTriangleArea(P1, P4, P6)
                            mesh_face_t2_area = getTriangleArea(P2, P5, P4)
                            mesh_face_t3_area = getTriangleArea(P3, P6, P5)
                            mesh_face_t4_area = getTriangleArea(P4, P5, P6)
                            mesh_face_area = mesh_face_t1_area + mesh_face_t2_area + mesh_face_t3_area + mesh_face_t4_area
                            middle_node_area = mesh_face_area / 3.0

                            node_area_table.append((face_table[mf][0], 0))
                            node_area_table.append((face_table[mf][1], 0))
                            node_area_table.append((face_table[mf][2], 0))
                            node_area_table.append((face_table[mf][3], middle_node_area))
                            node_area_table.append((face_table[mf][4], middle_node_area))
                            node_area_table.append((face_table[mf][5], middle_node_area))

                        elif len(face_table[mf]) == 8:  # 8 node mesh face quad
                            FreeCAD.Console.PrintError('Face load on 8 node quad faces are not supported\n')

                    # node_sumarea_table
                    for n, A in node_area_table:
                        # print(n, ' --> ', A)
                        if n in node_sumarea_table:
                            node_sumarea_table[n] = node_sumarea_table[n] + A
                        else:
                            node_sumarea_table[n] = A

                    sum_node_areas = 0
                    for n in node_sumarea_table:
                        sum_node_areas = sum_node_areas + node_sumarea_table[n]
                    sum_ref_face_node_area += sum_node_areas

                    # write CLOAD lines to CalculiX file
                    vec = frc_obj.DirectionVector
                    for n in sorted(node_sumarea_table):
                        node_load = node_sumarea_table[n] * force_per_sum_ref_face_area
                        sum_node_load += node_load
                        if (vec.x != 0.0):
                            v1 = "{:.13E}".format(vec.x * node_load)
                            f.write(str(n) + ',1,' + v1 + '\n')
                        if (vec.y != 0.0):
                            v2 = "{:.13E}".format(vec.y * node_load)
                            f.write(str(n) + ',2,' + v2 + '\n')
                        if (vec.z != 0.0):
                            v3 = "{:.13E}".format(vec.z * node_load)
                            f.write(str(n) + ',3,' + v3 + '\n')
                f.write('\n')
            f.write('\n')

    def write_constraints_pressure(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Element + CalculiX face + load in [MPa]\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        for fobj in self.pressure_objects:
            prs_obj = fobj['Object']
            f.write('*DLOAD\n')
            for o, e in prs_obj.References:
                rev = -1 if prs_obj.Reversed else 1
                elem = o.Shape.getElement(e)
                if elem.ShapeType == 'Face':
                    v = self.mesh_object.FemMesh.getccxVolumesByFace(elem)
                    f.write("** Load on face {}\n".format(e))
                    for i in v:
                        f.write("{},P{},{}\n".format(i[0], i[1], rev * prs_obj.Pressure))

    def write_frequency(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Frequency analysis\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        f.write('*FREQUENCY\n')
        f.write('{},{},{}\n'.format(self.no_of_eigenfrequencies, self.eigenfrequeny_range_low, self.eigenfrequeny_range_high))

    def write_outputs_types(self, f):
        f.write('\n***********************************************************\n')
        f.write('** Outputs --> frd file\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        if self.beamsection_objects or self.shellthickness_objects:
            f.write('*NODE FILE, OUTPUT=2d\n')
        else:
            f.write('*NODE FILE\n')
        f.write('U\n')
        f.write('*EL FILE\n')
        f.write('S, E\n')
        f.write('** outputs --> dat file\n')
        f.write('*NODE PRINT , NSET=Nall \n')
        f.write('U \n')
        f.write('*EL PRINT , ELSET=Eall \n')
        f.write('S \n')

    def write_step_end(self, f):
        f.write('\n***********************************************************\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        f.write('*END STEP \n')

    def write_footer(self, f):
        f.write('\n***********************************************************\n')
        f.write('** CalculiX Input file\n')
        f.write('** written by {} function\n'.format(sys._getframe().f_code.co_name))
        f.write('**   written by    --> FreeCAD ' + self.fc_ver[0] + '.' + self.fc_ver[1] + '.' + self.fc_ver[2] + '\n')
        f.write('**   written on    --> ' + time.ctime() + '\n')
        f.write('**   file name     --> ' + os.path.basename(FreeCAD.ActiveDocument.FileName) + '\n')
        f.write('**   analysis name --> ' + self.analysis.Name + '\n')
        f.write('**\n')
        f.write('**\n')
        f.write('**\n')
        f.write('**   Units\n')
        f.write('**\n')
        f.write('**   Geometry (mesh data)        --> mm\n')
        f.write("**   Materials (Young's modulus) --> N/mm2 = MPa\n")
        f.write('**   Loads (nodal loads)         --> N\n')
        f.write('**\n')

    # self.ccx_elsets = [ {
    #                        'beamsection_obj' : 'beamsection_obj'       if exists
    #                        'shellthickness_obj' : shellthickness_obj'  if exists
    #                        'ccx_elset' : [e1, e2, e3, ... , en] or string self.ccx_eall
    #                        'ccx_elset_name' : 'ccx_identifier_elset'
    #                        'mat_obj_name' : 'mat_obj.Name'
    #                        'ccx_mat_name' : 'mat_obj.Material['Name'][:80]'   !!! not unique !!!
    #                     },
    #                     {}, ... , {} ]
    def get_ccx_elsets_single_mat_single_beam(self):
        mat_obj = self.material_objects[0]['Object']
        beamsec_obj = self.beamsection_objects[0]['Object']
        ccx_elset = {}
        ccx_elset['beamsection_obj'] = beamsec_obj
        ccx_elset['ccx_elset'] = self.ccx_eall
        ccx_elset['ccx_elset_name'] = get_ccx_elset_beam_name(mat_obj.Name, beamsec_obj.Name)
        ccx_elset['mat_obj_name'] = mat_obj.Name
        ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
        self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_single_mat_single_shell(self):
        mat_obj = self.material_objects[0]['Object']
        shellth_obj = self.shellthickness_objects[0]['Object']
        ccx_elset = {}
        ccx_elset['shellthickness_obj'] = shellth_obj
        ccx_elset['ccx_elset'] = self.ccx_eall
        ccx_elset['ccx_elset_name'] = get_ccx_elset_shell_name(mat_obj.Name, shellth_obj.Name)
        ccx_elset['mat_obj_name'] = mat_obj.Name
        ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
        self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_single_mat_solid(self):
        mat_obj = self.material_objects[0]['Object']
        ccx_elset = {}
        ccx_elset['ccx_elset'] = self.ccx_eall
        ccx_elset['ccx_elset_name'] = get_ccx_elset_solid_name(mat_obj.Name)
        ccx_elset['mat_obj_name'] = mat_obj.Name
        ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
        self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_single_mat_multiple_beam(self):
        mat_obj = self.material_objects[0]['Object']
        self.get_femelement_sets(self.beamsection_objects)
        for beamsec_data in self.beamsection_objects:
            beamsec_obj = beamsec_data['Object']
            ccx_elset = {}
            ccx_elset['beamsection_obj'] = beamsec_obj
            ccx_elset['ccx_elset'] = beamsec_data['FEMElements']
            ccx_elset['ccx_elset_name'] = get_ccx_elset_beam_name(mat_obj.Name, beamsec_obj.Name, None, beamsec_data['ShortName'])
            ccx_elset['mat_obj_name'] = mat_obj.Name
            ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
            self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_single_mat_multiple_shell(self):
        mat_obj = self.material_objects[0]['Object']
        self.get_femelement_sets(self.shellthickness_objects)
        for shellth_data in self.shellthickness_objects:
            shellth_obj = shellth_data['Object']
            ccx_elset = {}
            ccx_elset['shellthickness_obj'] = shellth_obj
            ccx_elset['ccx_elset'] = shellth_data['FEMElements']
            ccx_elset['ccx_elset_name'] = get_ccx_elset_shell_name(mat_obj.Name, shellth_obj.Name, None, shellth_data['ShortName'])
            ccx_elset['mat_obj_name'] = mat_obj.Name
            ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
            self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_multiple_mat_single_beam(self):
        beamsec_obj = self.beamsection_objects[0]['Object']
        self.get_femelement_sets(self.material_objects)
        for mat_data in self.material_objects:
            mat_obj = mat_data['Object']
            ccx_elset = {}
            ccx_elset['beamsection_obj'] = beamsec_obj
            ccx_elset['ccx_elset'] = mat_data['FEMElements']
            ccx_elset['ccx_elset_name'] = get_ccx_elset_beam_name(mat_obj.Name, beamsec_obj.Name, mat_data['ShortName'])
            ccx_elset['mat_obj_name'] = mat_obj.Name
            ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
            self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_multiple_mat_single_shell(self):
        shellth_obj = self.shellthickness_objects[0]['Object']
        self.get_femelement_sets(self.material_objects)
        for mat_data in self.material_objects:
            mat_obj = mat_data['Object']
            ccx_elset = {}
            ccx_elset['shellthickness_obj'] = shellth_obj
            ccx_elset['ccx_elset'] = mat_data['FEMElements']
            ccx_elset['ccx_elset_name'] = get_ccx_elset_shell_name(mat_obj.Name, shellth_obj.Name, mat_data['ShortName'])
            ccx_elset['mat_obj_name'] = mat_obj.Name
            ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
            self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_multiple_mat_solid(self):
        self.get_femelement_sets(self.material_objects)
        for mat_data in self.material_objects:
            mat_obj = mat_data['Object']
            ccx_elset = {}
            ccx_elset['ccx_elset'] = mat_data['FEMElements']
            ccx_elset['ccx_elset_name'] = get_ccx_elset_solid_name(mat_obj.Name, None, mat_data['ShortName'])
            ccx_elset['mat_obj_name'] = mat_obj.Name
            ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
            self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_multiple_mat_multiple_beam(self):
        self.get_femelement_sets(self.beamsection_objects)
        self.get_femelement_sets(self.material_objects)
        for beamsec_data in self.beamsection_objects:
            beamsec_obj = beamsec_data['Object']
            for mat_data in self.material_objects:
                mat_obj = mat_data['Object']
                ccx_elset = {}
                ccx_elset['beamsection_obj'] = beamsec_obj
                elemids = []
                for elemid in beamsec_data['FEMElements']:
                    if elemid in mat_data['FEMElements']:
                        elemids.append(elemid)
                ccx_elset['ccx_elset'] = elemids
                ccx_elset['ccx_elset_name'] = get_ccx_elset_beam_name(mat_obj.Name, beamsec_obj.Name, mat_data['ShortName'], beamsec_data['ShortName'])
                ccx_elset['mat_obj_name'] = mat_obj.Name
                ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
                self.ccx_elsets.append(ccx_elset)

    def get_ccx_elsets_multiple_mat_multiple_shell(self):
        self.get_femelement_sets(self.shellthickness_objects)
        self.get_femelement_sets(self.material_objects)
        for shellth_data in self.shellthickness_objects:
            shellth_obj = shellth_data['Object']
            for mat_data in self.material_objects:
                mat_obj = mat_data['Object']
                ccx_elset = {}
                ccx_elset['shellthickness_obj'] = shellth_obj
                elemids = []
                for elemid in shellth_data['FEMElements']:
                    if elemid in mat_data['FEMElements']:
                        elemids.append(elemid)
                ccx_elset['ccx_elset'] = elemids
                ccx_elset['ccx_elset_name'] = get_ccx_elset_shell_name(mat_obj.Name, shellth_obj.Name, mat_data['ShortName'], shellth_data['ShortName'])
                ccx_elset['mat_obj_name'] = mat_obj.Name
                ccx_elset['ccx_mat_name'] = mat_obj.Material['Name'][:80]
                self.ccx_elsets.append(ccx_elset)

    def get_femelement_sets(self, fem_objects):
        # get femelements for reference shapes of each obj.References
        if not hasattr(self, 'fem_element_table'):
            self.fem_element_table = getFemElementTable(self.mesh_object.FemMesh)
        count_femelements = 0
        referenced_femelements = []
        has_remaining_femelements = None
        for fem_object_i, fem_object in enumerate(fem_objects):
            obj = fem_object['Object']
            fem_object['ShortName'] = get_ccx_elset_short_name(obj, fem_object_i)  # unique short ccx_identifier
            if obj.References:
                ref_shape_femelements = []
                for ref in obj.References:
                    femnodes = []
                    femelements = []
                    r = ref[0].Shape.getElement(ref[1])
                    print('  ReferenceShape : ', r.ShapeType, ', ', ref[0].Name, ', ', ref[0].Label, ' --> ', ref[1])
                    if r.ShapeType == 'Edge':
                        femnodes = self.mesh_object.FemMesh.getNodesByEdge(r)
                    elif r.ShapeType == 'Face':
                        femnodes = self.mesh_object.FemMesh.getNodesByFace(r)
                    elif r.ShapeType == 'Solid':
                        # femnodes = self.mesh_object.FemMesh.getNodesBySolid(r)  -->  TODO
                        FreeCAD.Console.PrintError('Solid Reference Shapes, CalculiX input file may be broken!\n')
                        fem_object['FEMElements'] = self.ccx_eall
                        return
                    else:
                        print('  No Edge, Face or Solid as reference shapes!')
                    femelements = getFemElementsByNodes(self.fem_element_table, femnodes)
                    ref_shape_femelements += femelements
                    referenced_femelements += femelements
                    count_femelements += len(femelements)
                fem_object['FEMElements'] = ref_shape_femelements
            else:
                has_remaining_femelements = obj.Name
        # get remaining femelements for the fem_objects
        if has_remaining_femelements:
            remaining_femelements = []
            for elemid in self.fem_element_table:
                if elemid not in referenced_femelements:
                    remaining_femelements.append(elemid)
            count_femelements += len(remaining_femelements)
            for fem_object in fem_objects:
                obj = fem_object['Object']
                if obj.Name == has_remaining_femelements:
                    fem_object['FEMElements'] = sorted(remaining_femelements)
        # check if all worked out well
        if not femelements_count_ok(self.fem_element_table, count_femelements):
            FreeCAD.Console.PrintError('Error in get_femelement_sets -- > femelements_count_ok failed!\n')


# Helpers
def getTriangleArea(P1, P2, P3):
    vec1 = P2 - P1
    vec2 = P3 - P1
    vec3 = vec1.cross(vec2)
    return 0.5 * vec3.Length


def getFemElementTable(fem_mesh):
    """ getFemElementTable(fem_mesh): { elementid : [ nodeid, nodeid, ... , nodeid ] }"""
    fem_element_table = {}
    if is_solid_mesh(fem_mesh):
        for i in fem_mesh.Volumes:
            fem_element_table[i] = fem_mesh.getElementNodes(i)
    elif is_shell_mesh(fem_mesh):
        for i in fem_mesh.Faces:
            fem_element_table[i] = fem_mesh.getElementNodes(i)
    elif is_beam_mesh(fem_mesh):
        for i in fem_mesh.Edges:
            fem_element_table[i] = fem_mesh.getElementNodes(i)
    else:
        FreeCAD.Console.PrintError('Neither solid nor shell nor beam mesh!\n')
    return fem_element_table


def getFemElementsByNodes(fem_element_table, node_list):
    '''if all nodes of an fem_element are in node_list,
    the fem_element is added to the list which is returned
    e: elementlist
    nodes: nodelist '''
    e = []  # elementlist
    for elementID in sorted(fem_element_table):
        nodecount = 0
        for nodeID in fem_element_table[elementID]:
            if nodeID in node_list:
                nodecount = nodecount + 1
        if nodecount == len(fem_element_table[elementID]):   # all nodes of the element are in the node_list!
            e.append(elementID)
    return e


def is_solid_mesh(fem_mesh):
    if fem_mesh.VolumeCount > 0:  # solid mesh
        return True


def has_no_face_data(fem_mesh):
    if fem_mesh.FaceCount == 0:   # mesh has no face data, could be a beam mesh or a solid mesh without face data
        return True


def is_shell_mesh(fem_mesh):
    if fem_mesh.VolumeCount == 0 and fem_mesh.FaceCount > 0:  # shell mesh
        return True


def is_beam_mesh(fem_mesh):
    if fem_mesh.VolumeCount == 0 and fem_mesh.FaceCount == 0 and fem_mesh.EdgeCount > 0:  # beam mesh
        return True


def femelements_count_ok(fem_element_table, count_femelements):
    if count_femelements == len(fem_element_table):
        # print('Count Elements written to CalculiX file: ', count_femelements)
        # print('Count Elements of the FreeCAD FEM Mesh:  ', len(fem_element_table))
        return True
    else:
        print('ERROR: self.fem_element_table != count_femelements')
        print('Count Elements written to CalculiX file: ', count_femelements)
        print('Count Elements of the FreeCAD FEM Mesh:  ', len(fem_element_table))
        return False


def get_ccx_elset_beam_name(mat_name, beamsec_name, mat_short_name=None, beamsec_short_name=None):
    if not mat_short_name:
        mat_short_name = 'Mat0'
    if not beamsec_short_name:
        beamsec_short_name = 'Beam0'
    if len(mat_name + beamsec_name) > 20:   # max identifier lenght in CalculiX for beam elsets
        return mat_short_name + beamsec_short_name
    else:
        return mat_name + beamsec_name


def get_ccx_elset_shell_name(mat_name, shellth_name, mat_short_name=None, shellth_short_name=None):
    if not mat_short_name:
        mat_short_name = 'Mat0'
    if not shellth_short_name:
        shellth_short_name = 'Shell0'
    if len(mat_name + shellth_name) > 80:   # standard max identifier lenght in CalculiX
        return mat_short_name + shellth_short_name
    else:
        return mat_name + shellth_name


def get_ccx_elset_solid_name(mat_name, solid_name=None, mat_short_name=None):
    if not solid_name:
        solid_name = 'Solid'
    if not mat_short_name:
        mat_short_name = 'Mat0'
    if len(mat_name + solid_name) > 80:   # standard max identifier lenght in CalculiX
        return mat_short_name + solid_name
    else:
        return mat_name + solid_name


def get_ccx_elset_short_name(obj, i):
    if hasattr(obj, "Proxy") and obj.Proxy.Type == 'MechanicalMaterial':
        return 'Mat' + str(i)
    elif hasattr(obj, "Proxy") and obj.Proxy.Type == 'FemBeamSection':
        return 'Beam' + str(i)
    elif hasattr(obj, "Proxy") and obj.Proxy.Type == 'FemShellThickness':
        return 'Shell' + str(i)
    else:
        print 'Error: ', obj.Name, ' --> ', obj.Proxy.Type