$$$$ G_THETA NOTICE BP208322 12/10/04 21:15:18 7519 DATE 12/10/04 Procedure G_THETA Voir aussi : CH_THETA ----------------- G_THETA TAB2 ; SUPTAB.'OBJECTIF' 'FRONT_FISSURE' 'LEVRE_SUPERIEURE' 'LEVRE_INFERIEURE' 'COUCHE' 'SOLUTION_PASAPAS' 'SOLUTION_RESO' 'CARACTERISTIQUES' 'MODELE' 'TEMPERATURES' 'BLOCAGES_MECANIQUES' 'MODELES_COMPOSITES' 'NOEUDS_AVANCES' 'FISSURE_2' 'FRONT_FISSURE_2' 'POINT_CENTRE' 'POINT_1' 'POINT_2' 'POINT_2' 'POINT_3' 'CHPOINT_TRANSFORMATION' 'OPERATEUR' 'CHAMP_THETA' 'ELEMENT_MULTICOUCHE' 'CALCUL_CRITERE' Description : °°°°°°°°°°°°° This procedure has two objectifs : 1 ) calculate some line integrals of fracture mechanics as follows : 1.1) the J line integral of an isotropic material, which characterizes the crack tip fields in elasto-plasticity. In 3D brick element case, composite materials are not yet acceptable. 1.2) the J line dynamic integral of an isotropic material, which characterizes the crack tip fields for elasto-dynamic problems. In 3D brick element case, composite materials are not yet acceptable. 1.3) the C* line integral of an isotropic material, which characterizes the crack tip fields in the case of secondary creep problems. Applied loadings must be mechanics and composite materials are not yet acceptable, neither in 2D configurations nor in 3D configurations. 1.4) the C*(h) line integral of an isotropic material, which characterizes the crack tip fields in the case of primary or tertiary creep problems. Applied loadings must be mechanics and composite materials are not yet acceptable, neither in 2D configurations nor in 3D configurations. 1.5) the derivative integral dJ/da (a : crack length) line integral of an isotropic homogeneous material, required in the stability analysis of a single crack or a system of interacting cracks. Only the brick elements (2D or 3D) are acceptable and composite materials are not yet available for calculating this derivative integral. 2 ) seperate the stress intensity factors K1, K2 (and K3 in 3D) for elastic problems in 2D, 3D (brick elements only) or axisymetrical configurations. For seperating a mixed mode, the current version of G_THETA procedure accepts only isotropic homogeneous materials. Contents : °°°°°°°°°° Input data of the procedure is a TABLE type object, SUPTAB, whose indexes are objects of MOT type, writen in capital case and described as follows : Arguments compulsory for all types of calculations : ___________________________________________________ SUPTAB.'OBJECTIF' = MOT type, specifying the calculation aim, egal to 1.1) 'J' for calculating the J line integral, characteristics in elasto-plasticity. 1.2) 'J-DYNA' for calculating the J dynamic line integral, characteristics in elasto- dynamic mechanics. 1.3) 'C*' for calculating the C* line integral, characteristics for secondary creep problems. 1.4) 'C*(h)' for calculating the C*(h) line integral, characteristics for primary or tertiary creep problems. 1.5) 'DJ/DA' for calculating the derivative dJ/da line integral, required in the analysis of crack growth stability analysis. 1.6) 'DECOUPLAGE' for seperating the the stress intensity factors K1, K2 (and K3 in 3D) for crack problems in mixed fracture mode. SUPTAB.'COUCHE' = ENTIER type. It is the number of layers of elements surrounding the crack tip in 2D (or surrounding a point on the crack front in 3D), that support the virtual crack extension. If COUCHE = 0, the THETA field equals 1 only at the crack tip (in 2D), or equals 1 for all points on the crack front (in 3D). In general, more the number of layers of elements is important, more the value calculated by the present G_THETA procedure is accurate. But the elements included in the number of layers should not attain mesh's border. SUPTAB.'FRONT_FISSURE' = POINT type in 2D or 3D shell element case, MAILLAGE type in 3D brick elements case. This object gives the front of the crack. Arguments compulsory for standard elements : ___________________________________________________ SUPTAB.'LEVRE_SUPERIEURE' = following the conventional definition, this object (MAILLAGE type) gives the crack's superior lip. SUPTAB.'LEVRE_INFERIEURE' = following the conventional definition, this object (MAILLAGE type) gives the crack's inferior lip. If only one of the lips is modeled, one of the words LEVRE_SUPERIEURE or LEVRE_INFERIEURE is sufticient to describe the entire crack. Arguments compulsory for XFEM elements : ___________________________________________________ SUPTAB.'PSI' = 1st level set function (CHPOINT) describing the crack SUPTAB.'PHI' = 2nd level set. Arguments compulsory for solutions by PASAPAS procedure _______________________________________________________ SUPTAB.'SOLUTION_PASAPAS' = TABLE resulting from PASAPAS procedure. Arguments compulsory for solutions by RESO operator ___________________________________________________ SUPTAB.'SOLUTION_RESO' = displacement solution (CHPOINT type) resulting from RESO operator. SUPTAB.'CARACTERISTIQUES' = MCHAML object of CARACTERISTIQUES subtype. In the case of calculations with shell elements, this object includes material's properties (Young's modulus, Poisson's coefficient ...) and geometrical parameters like shell's thincknees, generated by operator MATE or CARA. SUPTAB.'MODELE' = modele object (type MMODEL) including all structure. SUPTAB.'TEMPERATURES' = temperature (CHPOINT or MCHAML type) generating a thermal stresse non nul if it exists. SUPTAB.'CHARGEMENTS_MECANIQUES' = all external mechanical loadings (CHPOINT type) if they exist. SUPTAB.'BLOCAGES_MECANIQUES' = RIGIDITE type representing the mechanics blockading matrice of given problem. Optional arguments __________________ 1 : Composite material case (2D brick or 3D shell element only) SUPTAB.'MODELES_COMPOSITES' = TABLE type whose index is 1, 2, 3,..., n. n is the number of MMODEL objects having discontinue material or geometrical properties. 2 : For a 3D crack front SUPTAB.'NOEUDS_AVANCES' = POI1 type, giving points on the crack front for which the calculations will be performed. 3 : Calculation of the termes dJi/daj (i is not egal to j) in the cas of interacting case SUPTAB.'FISSURE_2' = MAILLAGE type representing another crack (superior lip + inferior lip if all two lips are present). SUPTAB.'FRONT_FISSURE_2' = POINT ou MAILLAGE type representing the tip of the crack 2 described above. 4 : Circular crack in a plan configuration (2D) SUPTAB.'POINT_CENTRE' = POINT type, giving the center of the circular crack. 5 : Crack in a straight pipe (3D) SUPTAB.'POINT_1' = POINT type, giving the center of the coordinates system. SUPTAB.'POINT_2' = POINT type. POINT_1 to POINT_2 constitutes the positive direction of Z axis. SUPTAB.'POINT_3' = POINT type. POINT_1, POINT_2 and POINT_3 constitute the surface which defines theta angle equal to zero. 6 : Crack in the elbow of a pipe (3D) SUPTAB.'POINT_1' = POINT type SUPTAB.'POINT_2' = POINT type. For a crack tip, POINT_1 and POINT_2 constitute a rotation axe for the crack. SUPTAB.'CHPOINT_TRANSFORMATION' = CHPOINT type, used for transforming an elbow into a straight pipe by using operator 'PLUS' or 'MOIN'. SUPTAB.'OPERATEUR' = MOT type. Its value is 'PLUS' or 'MOIN' to indicate the use of operator PLUS or MOIN for transforming the elbow into a straight pipe. 7 : Rigid rotation given in the calculations by PASAPAS SUPTAB.'ROTATION_RIGIDIFIANTE' = TABLE type whose index is 0,1,2... in order to provide the displacement field due to the rigid rotation of the structure arround a point. This rotation is declaimed as an input of the PASAPAS procudure when performing a calculation with great displacement. 8 : Theta field provided by user himself SUPTAB.'CHAMP_THETA' = CHPOINT type, simulating the virtual crack growth. Caution : if half-specimen modeling (due to symetry in the crack plane), the norm of theta field shoudl vary from 2. to 0. (instead of from 1. to 0. in the case of full specimen modeling). 9 : Case where one wants to calculate a line integral along any 3D crack front modeled by shell elements (report DMT/96-317) For this purpose we can use the multilayer technique which consists, before the call of G_THETA procedure, in : 1) Establishing a multilayer model (cf MODE CONS) for one or sevral element(s) near the crack tip. These elements should be neither too close to the crack tip, nor too far from it for the reason of calculation accuracy. At least three multilayers must be established, respectively in crack's inferior level, middle level and superior level. These layers must have thickness less 1e-4*(total shell thickness). Taking into account the intermediate layers betweent the thin multilayers, there must be at least five layers in the thickness direction of shell element. 2) giving an exccentricity and a different constituent name for all layers in shell elements. 3) assembling the resulting multilayer models with the model objet established for the other monolayer elements. 4) performing the stress-strain calculations with the total mecanical model and the total meterial characteristics including all structure. Then, the calculation of the line integral using the G_THETA procedure will be done for A SINGLE element and for all its thin layers having a thickness less than 1e-4*(total shell thickness).This multilayer element should be specified thoughout an argument as follows : SUPTAB.'ELEMENT_MULTICOUCHE' = MAILLAGE objet including A SINGLE multilayer element. It should be situated in the THETA region, i.e. a crack-tip-near zone defined by the number, SUPTAB.'COUCHE', which indicates the number of circular element rows from the crack tip to support the virtual crack extensions. For the reason of computation accuracy, this element should be neither too close to the crack tip, nor too far from it. Theoritically, the value of the line integral is independent of the selecion of such a multilayer element. Numerically, this point is verifiable by computing the integral with different multilayer element in a serie of G_THETA callings. Note however that the presented multilayer method needs a mesh model very fine in the crack type region. 10 : If we want the calculation of criteria for proportionnal loading SUPTAB.'CALCUL_CRITERE' = BOOLEAN VRAI if we want the calculation, FAUX if we don't want the calculati (default value = VRAI) Output data °°°°°°°°°°° The results corresponding to a THETA field specified by the SUPTAB.'COUCHE' object (or SUPTAB.'CHAMP_THETA' object in the case where user want to give himself a THETA field) are stored in the following manner : In all calculation case ----------------------- SUPTAB.'CHPO_RESULTATS' = CHPOINT object numerical result of the computation supported by the crack front (or TABLE of CHPOINT results organised like SUPTAB.'RESULTATS'). SUPTAB.'RESULTATS' = Object containing the numerical value of calculations. Its type is variable, depending on the problem configuration (2D or 3D) and the solutions provided (PASAPAS or RESO) : 1) value of a line integral in the case of a solution come from RESO operator 2D => FLOTTANT 3D brick => TABLE indexed by .(points on the crack front) and .'GLOBAL' for a global estimation 3D sheel => TABLE indexed by words (MOT type) .'SUPERI' on the superior layer of sheel .'INFERI' on the inferior layer of sheel .'MEDIAN' on the middle plan of sheel .'GLOBAL' for a global estimation 2) value of a line integral in the case of a solution come from PASAPAS procedure 2D => TABLE indexed by .(calculation step number) 3D brick => TABLE indexed by .(calculation step number).(points on the crack front) and .(calculation step number).'GLOBAL' for a global estimation 3D sheel => TABLE indexed by .(calculation step number).'SUPERI' .(calculation step number).'INFERI' .(calculation step number).'MEDIAN' and .(calculation step number).'GLOBAL' 3) value of stresse intensity factors S.I.C. in the case of seperation of mixed mode fracture with a solution come from RESO operator 2D => TABLE indexed by words (MOT type) .'I' for the value of KI .'II' for the value of KII 3D brick => TABLE indexed by .'I' .(points on the crack front) and .'I' .'GLOBAL' for the value of KI .'II' .(points on the crack front) and .'II' .'GLOBAL' for the value of KII .'III'.(points on the crack front) and .'III'.'GLOBAL' for the value of KIII 4) value of stresse intensity factors S.I.C. in the case of seperation of mixed mode fracture with a solution come from PASAPAS procedure 2D => TABLE indexed by .'I' .(calculation step number) for the value of KI .'II'.(calculation step number) for the value of KII 3D brick => TABLE indexed by .'I' .(calculation step number).(points on the crack front) and .'I' .(calculation step number).'GLOBAL' .'II' .(calculation step number).(points on the crack front) and .'II' .(calculation step number).'GLOBAL' .'III'.(calculation step number).(points on the crack front) and .'III'.(calculation step number).'GLOBAL' Solution come from PASAPAS procedure ------------------------------------ SUPTAB.'EVOLUTION_RESULTATS' = Object representing the variation of computed results in the fonction of time evolution. Its type is variable, depending on the problem configuration (2D or 3D) : 1) Time evolution of a line integral 2D => EVOLUTION type 3D brick => TABLE indexed by .(points on the crack front) .'GLOBAL' time evolution for a global estimation 3D sheel => TABLE indexed by words .'SUPERI' time evolution of values on the sheel superior layer .'INFERI' time evolution of values on the sheel inferior layer .'MEDIAN' time evolution of values on the sheel middle plan .'GLOBAL' time evolution of a global estimation 2) Time evolution of stresse intensity factors (S.I.F.) 2D => TABLE indexed by words .'I' for KI evolution .'II' for KII evolution 3D brick => TABLE indexed by .'I'. (points on the crack front) and .'I'. 'GLOBAL' for KI evolution .'II'. (points on the crack front) and .'II'. 'GLOBAL' for KII evolution .'III'.(points on the crack front) and .'III'.'GLOBAL' for KIII evolution Calculations with sheel elements -------------------------------- SUPTAB.'EPAISSEUR_RESULTATS' = object representing the variation of computed value of a line integral in the sheel's thicknees direction. Its type is variable, depending on the solution given : 1) EVOLUTION in the case of a solution coming from RESO operator 2) TABLE indexed by .(calculation step number) in the case of a solution coming from PASAPAS procedure. Calculations in elasto-plasticity --------------------------------- In case of ELASTIQUE PLASTIQUE material, ISOTROPE or CINEMATIQUE, possibly THERMIQUE : SUPTAB.'CRIT_DECHA_GLOBAL1' = We evaluate a critetion of decreasing of the stresses defined by (if, F = tension curve): crit = F(STRAINeq)/ STRESSeq. crit = 1 if no-decreasing and crit > 1 if decreasing. SUPTAB.'CRITERE_DECHARGE' is a TABLE type object indexed by the calculation step containing INTEGERs. SUPTAB.'CRIT_DECHA_GLOBAL2' = We evaluate a critetion of decreasing and the change of direction of the stresses using : crit = 2 - SIG:EPSpl/SIGeq_max.EPSE. if no-decrease and no-change of direction crit=1 and crit > 1. in different cases. SUPTAB.'CRIT_DECHA_GLOBAL2' is a TABLE type objec indexed by the calculation step containing INTEGERs. SUPTAB.'CRIT_DECHA_LOCAL1' = We evaluate a critetion of decreasing of the stresses using : crit = (delta SIG)/SIG crit = 0. if no-decrease and crit > 0. if decreas SUPTAB.'CRIT_DECHA_LOCAL1' is a TABLE type object indexed by the calculation step containing CHPOINT type objects. SUPTAB.'CRIT_DECHA_LOCAL2' = We evaluate a critetion for the change of direction of the stresses using : crit = SIG:(delta SIG)/norme(SIG).norme(delta SI crit = 1. if no-change of direction and crit = -1. if stresses are in opposite direction SUPTAB.'CRIT_DECHA_LOCAL2' is a TABLE type objec indexed by the calculation step containing CHPOINT type objects. Remark : °°°°°°°° The table SUPTAB also contains other objects used for resuming calculations; this table should be saved for resumimg a later calculation. Since the results are located in SUPTAB this procedure does not create any other object.
© Cast3M 2003 - All rights reserved.
Disclaimer