CN107145651B - ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file - Google Patents
ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file Download PDFInfo
- Publication number
- CN107145651B CN107145651B CN201710270976.4A CN201710270976A CN107145651B CN 107145651 B CN107145651 B CN 107145651B CN 201710270976 A CN201710270976 A CN 201710270976A CN 107145651 B CN107145651 B CN 107145651B
- Authority
- CN
- China
- Prior art keywords
- infinite
- inp
- unit
- boundary
- node
- Prior art date
- Legal status (The legal status is an assumption and is not a legal conclusion. Google has not performed a legal analysis and makes no representation as to the accuracy of the status listed.)
- Expired - Fee Related
Links
Images
Classifications
-
- G—PHYSICS
- G06—COMPUTING; CALCULATING OR COUNTING
- G06F—ELECTRIC DIGITAL DATA PROCESSING
- G06F30/00—Computer-aided design [CAD]
- G06F30/20—Design optimisation, verification or simulation
- G06F30/23—Design optimisation, verification or simulation using finite element methods [FEM] or finite difference methods [FDM]
-
- G—PHYSICS
- G06—COMPUTING; CALCULATING OR COUNTING
- G06F—ELECTRIC DIGITAL DATA PROCESSING
- G06F2111/00—Details relating to CAD techniques
- G06F2111/10—Numerical modelling
Landscapes
- Engineering & Computer Science (AREA)
- Physics & Mathematics (AREA)
- Theoretical Computer Science (AREA)
- Computer Hardware Design (AREA)
- Evolutionary Computation (AREA)
- Geometry (AREA)
- General Engineering & Computer Science (AREA)
- General Physics & Mathematics (AREA)
- Information Retrieval, Db Structures And Fs Structures Therefor (AREA)
Abstract
The invention discloses an ABAQUS three-dimensional infinite element boundary rapid modeling method based on an INP file, which belongs to the field of infinite unit boundary modeling. The method is simple to operate, the ABAQUS infinite element boundary model can be generated in a short time, and the modeling rate of the ABAQUS is greatly improved.
Description
Technical Field
The invention relates to an infinite unit boundary modeling method, in particular to an ABAQUS three-dimensional infinite element boundary rapid modeling method based on an INP file.
Background
The advent and rapid development of computers have provided powerful tools for engineering analysis, making it possible to solve many large-scale engineering practical problems using numerical simulations. The finite element method is used as the most common numerical simulation means and is widely applied to the engineering fields of rock and soil, structures, earthquakes, water conservancy and the like. The problem of using finite element method is how to use finite model to simulate real infinite area, the common solution is to neglect the influence of infinite area boundary according to Saint-Venn principle, use truncation boundary to take large enough model size to divide finite element mesh of geometric size, and apply corresponding approximate constraint boundary condition on artificial boundary. In actual calculation, the size identification of the model which is large enough is difficult, the calculation cost is low when the area is small, but the result precision is poor; when the area is large, certain precision requirements are met, but the calculation cost is high. Especially for the wave computation problem, the finite element computation results are often distorted by reflections and scattering of the wave at the mesh boundaries.
The reasonable artificial boundary is established by introducing the boundary unit, so that the reflection of the finite element boundary on the boundary of various fluctuations in the foundation caused by artificial truncation can be reduced as much as possible, the number of units is greatly reduced, and the calculation efficiency is improved. Currently, artificial boundaries such as viscous boundaries, paraxial approximation boundaries, transmission boundaries, viscoelastic boundaries, infinite element boundaries, and the like are common.
As a mode for simulating an infinite area, the appearance of an infinite element provides an important way for overcoming the defects of a finite element calculation method and solving the problem of infinite area boundary simulation. Infinite elements are an extension of finite elements in concept, and the main idea is to simulate an infinite physical field by geometrically bounding a "finite" element of infinite size. Also, since the infinite element must reflect the boundary characteristics of the near field or combine with finite elements that model the near field, it tends to be infinite in one direction only, and is therefore also referred to as a semi-infinite element. Infinite elements still fall into the category of finite elements in the broad finite element concept. In summary, infinite element is proposed to overcome the problem of infinite domain in finite element, and is often used to solve more complicated infinite problem with the conventional finite element, which is a supplement to finite element method, so it is more advantageous than other numerical methods such as boundary element to solve infinite domain problem.
A large number of experience in solving the infinite domain problem has shown that: the finite element and infinite element coupling model has wide practicability in solving the practical engineering problem. In particular, in the research of the problem of endogenous fluctuation, such as train vibration and explosion, and the seismic dynamics problem of exogenous vibration, infinite elements show obvious superiority in simulating and approximately simulating infinite domain problems. In addition, the finite element and infinite element coupling model is widely applied to the fields of electromagnetism, thermodynamics, acoustics and the like, and obtains good simulation effect. A plurality of infinite unit types are improved in large-scale finite element calculation software ABAQUS and ANSYS, and the infinite domain problem of finite element calculation is simulated. The ABAQUS is widely applied to power calculation in the field of geotechnical engineering by the powerful power nonlinear calculation capability.
ABAQUS provides first-order and second-order infinite elements including plane strain, plane stress, axisymmetric and three-dimensional infinite element elements, which are based on static calculation components such as ZienkiewiczThe simulation method is developed by dynamic response analysis such as Lysmer and the like, can be used for solving the problem of static infinite domain and solving the problem of local source vibration in the domain as an infinite element dynamic artificial boundary, namely, the simulation of external traveling waves which penetrate through the artificial boundary from the finite domain to the infinite domain is effective, and the problem of external source incidence is successfully solved by carrying out secondary development on the basis of ABAQUS infinite elements. Three-dimensional infinite units common to ABAQUS infinite element power artificial boundaries include CIN3D8, CIN3D12R(S)And CIN3D18R (S), etc., which may be combined with standard finite elements to simulate the near field region with finite elements and the far field region with infinite elements.
Although the ABAQUS boundary infinite unit provides convenience for static infinite element and dynamic artificial boundary simulation. However, since the node number in the infinite element ensures that the first surface of the element is the interface of the finite element and the infinite element to ensure the directivity of the infinite element, the extending direction of the element is from the near field to the far field. An infinite unit cannot be directly defined in the ABAQUS, only an infinite element boundary part can be preset during modeling, other unit types are adopted for distinguishing, the infinite element boundary part is exported to an ABAQUS input file (. inp), and then the comparison model manually modifies the unit node sequence of the infinite element boundary of the ABAQUS input file (. inp). Particularly for a three-dimensional boundary infinite unit, the modification process is complicated, more manpower and time are consumed especially when the analysis task amount is large, and a situation that manual operation errors cause grid operation errors often occurs.
The invention content is as follows:
the invention aims to solve the technical problem of providing an ABAQUS three-dimensional infinite element boundary rapid modeling method based on an INP file, overcoming the defects of complicated modeling process and low modeling efficiency of the conventional boundary infinite element model of the ABAQUS, considering the characteristics of ABAQUS infinite elements and the characteristics of ABAQUS input INP file model definition, having simple operation and high automation degree, generating infinite element grids in a short time and greatly improving the modeling efficiency of the ABAQUS.
In order to solve the technical problems, the invention adopts the technical scheme that:
according to a unit node definition rule in an ABAQUS three-dimensional infinite unit (3D infinite element), a unit and node definition method of an ABAQUS input file (. INP) is utilized, a data line defined by the ABAQUS infinite unit is output by means of Python, an input file defined by a model is completed according to a syntax rule of an INP file, and the ABAQUS/CAE is imported to generate a boundary infinite unit.
The technical scheme adopted by the invention for solving the technical problem comprises the following steps:
establishing a finite element model, establishing a specified Part boundary node set as a near field node set of an infinite element, and exporting an ABAQUS input file (Job-1. inp);
modifying the INP file to define a far-field node of an infinite unit by using a keyword (NCOPY) and storing the remote node as a new INP file (Job-2. INP);
Abaqus/CAE imports the modified INP file (Job-2.INP), looks up the generated infinite element far-field node and exports a new INP file (Job-3. INP);
an InP file (Job-3.INP) is specified, a keyword line ([ ELEMENT ]) is inserted into a position to define an infinite unit, and the infinite unit is stored as Job-4. INP;
python programming constructs infinite element boundary unit definition data lines and inputs the infinite element boundary unit definition data lines into an input file (Job-4.INP) of ABAQUS or a specified INP file;
the INP file (Job-4.INP) is opened in a mode of importing the ABAQUS model, and the ABAQUS designates that Part three-dimensional infinite unit boundaries are automatically generated.
Further, the specific steps of establishing an infinite element near-field node set in the finite element model and exporting an ABAQUS input file (Job-1.inp) comprise:
establishing an ABAQUS/CAE three-dimensional finite element model, and establishing a node set on a boundary surface of a designated Part as a near-field node set of a corresponding boundary infinite element by using a set tool under a Part module according to a research problem, namely four nodes on a first surface of the infinite element;
the analysis task Job-1 was created under the Job Module for the model of the problem and the ABAQUS Input file (Job-1.inp) was exported on Job Manager via Write Input.
Modifying the INP file to generate an infinite element far-field node by using the keyword ([ NCOPY ]), and storing the infinite element far-field node as the main content of a new INP file (Job-2.INP) comprises the following steps:
modifying the INP file Job-1.INP, and inserting a plurality of lines of keywords ([ NCOPY ]) defined by nodes in a specified Part definition line according to different boundary regions;
copying and shifting the near field nodes by using a keyword (NCOPY) to generate the far field nodes of different area boundary infinite elements;
storing the modified INP file as a new INP file (Job-2. INP);
the steps of importing the modified INP file Job-2.INP by Abaqus/CAE, checking the generated infinite element far-field node and exporting a new INP file Job-3.INP comprise:
importing the modified INP File Job-2.INP in a File → Import → Model manner through a graphical user interface GUI of Abaqus/CAE, wherein infinite elements of the far-field node are generated but cannot be displayed temporarily;
under the condition of a Part module, checking generated infinite element far-field nodes in different areas by clicking a Show node labels of Show node labels under View → Part Display Options → Mesh;
establishing a Job-3 task by the imported model in a Job module, and exporting a new INP file Job-3.INP through WriteInput on Job Manager;
the INP file Job-3.INP specifies the position to insert the keyword line ELEMENTS to define an infinite unit, and further includes for Job-4. INP:
editing an INP file Job-3.INP, and inserting a keyword line ELEMENT in a designated line to define an infinite unit;
and the INP file inserted with the ELEMENT keyword line and the data line is saved as a new INP file Job-4. INP.
Further, the main contents of the far-field node for generating infinite elements of different zone boundaries by copying and shifting the near-field node by using the keyword (. times.NCOPY) comprise:
the key word lines and data lines defined by the nodes must be edited according to the grammar rules of the INP file of ABAQUS;
new nodes are defined by NCOPY key rows and data rows.
Further, the key line and data line must be edited according to the syntax rules of the INP file of ABAQUS by the following steps:
1) the far-field node defines a Keyword Line (Keyword Line) as:
*NCOPY,CHANGE NUMBER＝N,OLD SET＝near_field_NodeSetName,NEW SET＝far_field_NodeSetName,SHIFT
2) the far-field node definition Data Line (Data Line) is:
Shifting-x,Shifting-y,Shifting-z
the key line and data line insertion position defined by the above nodes must be located before the definition End line End Part key of Part where the infinite element boundary is located, and behind the definition data line of the near field node set.
Defining a new node by NCOPY key line and data line mainly refers to:
copying and offsetting a certain distance through a near-field node, defining an infinite element boundary far-field node, and adding an integer value N to the node number of a new node on the basis of the original node number;
the near-field nodes and far-field nodes in the infinite element direction of the same infinite unit are in one-to-one correspondence, and the unit numbers have a difference of N;
the data line defines coordinate offset values of the newly created far-field node on the basis of the original near-field node.
Further, editing the INP file (Job-3.INP) and inserting a keyword (, ELEMENT) at a specific position to define details of an infinite ELEMENT means:
defining a new infinite cell by an ELEMENT key row and a data row;
the key word lines and data lines defined by the infinite unit must be edited according to the grammar rules of the INP file of ABAQUS;
the key line and data line insertion positions of the element definition must be located before the End-of-definition line End Part key of Part where the infinite element boundary is located, and the far-field node set definition data line and the finite element definition data line are located after.
Further, defining the specific content of the boundary infinite unit by the ELEMENT key word line and the data line includes:
the definition of the ABAQUS unit and the node is mainly to create a geometric shape and divide a unit grid through a preprocessor ABAQUS/CAE to form a unit node, wherein the ABAQUS infinite unit is defined in an INP file by manually editing the INP file, inserting an ELEMENT key word, assigning a unit number to the infinite unit, defining the unit through the specified unit node number, and simultaneously grouping the boundary infinite unit.
Considering that the unit number assigned on the ASSEMBLY (ASSEMBLY) is not unique, the combination Part (Part) is needed to distinguish, and the unit number assigned on the Part is unique, so the definition of the boundary infinite element is only defined on the designated Part;
an infinite unit is defined mainly through an ELEMENT keyword, the unit type is specified to be CIN3D8, and an infinite boundary ELEMENT set on a corresponding boundary area is established;
the data line defined by the infinite unit is a unit number and a node number formed by the units;
the data lines defined by the ABAQUS infinite cells can also be read from other INP files containing cell definition data;
the above-described node number arrangement order defined by the data line cell satisfies the node order defined by the three-dimensional infinite cell (CIN3D8) in the ABAQUS help document.
The key word line and data line defined by the infinite unit must be edited according to the grammar rule of INP file of ABAQUS, which specifically means that:
1) there are two ways for a Keyword Line (Keyword Line) defined by an infinite unit at an infinite unit boundary, which are respectively:
①*Element,type＝CIN3D8,Elset＝Infinite_Element_SetName
②*Element,type＝CIN3D8,Elset＝Infinite_Element_SetName,INPUT＝filename.inp
2) the corresponding infinite unit definition Data Line (Data Line) can correspond to the above key Line in two ways:
① the data line defined by the infinite element is directly inserted into the next line of the position of the infinite element definition key word of the corresponding area, which mainly comprises an infinite element number and a composition node number, namely:
Infinite_element_Num,NodeP1,NodeP2,NodeP3,NodeP4,NodeP5,NodeP6,NodeP7,NodeP8
② Inp, the file content is simply the line of data containing the current bounding area Infinity definition of the previous entry-including Infinity Unit number and component node number, i.e.:
Infinite_element_Num,NodeP1,NodeP2,NodeP3,NodeP4,NodeP5,NodeP6,NodeP7,NodeP8。
further, the data line Infinite _ element _ Num, node p1, node p2, node p3, node p4, node p5, node p6, node p7, node p8 defined by Infinite element include the following related conventions:
the node numbers of the four far field nodes of claims 5 and 6 are greater than the node number value of the corresponding near field node (node on finite element boundary) on the infinite direction element edge by N, that is:
according to the infinite unit definition rule, four nodes NodeP1, NodeP2, NodeP3 and NodeP4 in the near field of the first surface of the infinite unit are required to be arranged in a sequence of the four nodes in the near field in a counterclockwise direction when the four nodes are observed from the far field to the near field of the infinite unit;
the unit number designated by the infinite unit definition is determined by the number of finite units on the current Part, the number of infinite units in the defined boundary area and the order of the infinite unit definition in the area.
Further, the construction of the infinite element boundary unit definition data line by using Python programming and inputting the infinite element boundary unit definition data line into an input file (Job-4.INP) of the ABAQUS or a specified INP file specifically comprises the following steps:
1) reading a node number and a corresponding coordinate, a unit number and a component node number in an input file (Job-4.inp) of the ABAQUS by utilizing Python programming, and storing the node number and the corresponding coordinate, the unit number and the component node number in a specified list;
2) reading a key line number defined by an infinite unit in an INPUT file (Job-4.INP) of ABAQUS by utilizing Python programming and storing the key line number in a specified variable, or reading an INPUT parameter written by an infinite unit definition data line-the INP file.
3) Traversing the node list of the finite element model according to the characteristics of the node coordinates, searching nodes on different boundaries according to the characteristics of the coordinate values of the nodes of the boundaries, and adding the nodes to the specified boundary node list;
4) searching boundary units by traversing the unit list of the finite element model according to the relationship between the unit composition node coordinates and the characteristics of the node coordinates on the boundary, and adding the boundary units to the specified boundary unit list;
5) traversing the appointed boundary node list, taking out any four nodes A, B, C and D, and judging whether the four nodes are four nodes on the first surface of the boundary infinite unit near field;
6) if the four nodes A, B, C and D are four nodes on the first surface of the boundary infinite unit near field, solving a vector included angle relation according to the quantity product of the vectors to determine the relative position relation of the four nodes;
7) determining the arrangement sequence of the four nodes in the counterclockwise direction as Q1, Q2, Q3 and Q4 by using the vector product among the vectors;
8) the infinite unit serial number is determined by a Part unit number a specified in the finite model, a defined boundary infinite unit number b and an infinite unit definition sequence c in the region, and then the current infinite unit number is Q ═ a + b + c;
9) given a data line output specifying a boundary cell infinite element definition:
Q,Q1,Q2,Q3,Q4,Q1+N,Q2+N,Q3+N,Q4+N
wherein: q is an infinite element number, Q1, Q2, Q3, Q4 are four near-field nodes, Q1+ N, Q2+ N, Q3+ N, and Q4+ N are four far-field nodes;
10) two infinite unit definition data line output modes, wherein the former mainly adopts a key line ① and a data line ① aiming at infinite unit definition, namely the unit definition data line is directly inserted into the next line of the key definition position in Job-4.inp and is stored;
the latter mainly adopts a key line ② and a data line ② for the infinite unit definition, writes the data line of the unit definition into an INPUT parameter file.
Further, the specific steps of traversing the specified boundary node list, taking out any four nodes, and judging whether the node is four nodes on the first surface of the infinite meta-model near field are as follows:
by using the member test function of Python, if four nodes taken out from the boundary node list are four of the boundary unit composition nodes, the four nodes are considered as four near-field nodes on the first surface of the boundary infinite unit.
If the four nodes A, B, C and D are four nodes on the first surface of the boundary infinite unit near field, solving two vector included angles according to the vector quantity product to determine the relative position relation of the four nodes, and the specific steps comprise:
with point a as the first point of the quadrilateral, the sizes of ∠ BAC, <tttransition = & <t/t >tbad and ∠ CAD are respectively calculated using the vector quantity product and summed:
let SUM ∠ BAC + ∠ BAD + ∠ CAD:
1) if SUM is 2 ∠ BAC, point a and point D, point B and point C are diagonal nodes, and the counterclockwise direction of the nodes is a, B, D, C or a, C, D, B;
2) if SUM is 2 ∠ BAD, point a and point C, point B and point D are diagonal nodes to each other, and the counterclockwise direction of the nodes is sequentially a, B, C, D or a, D, C, B;
3) if SUM is 2 ∠ CAD, point a and point B, point C and point D are diagonal nodes to each other, and the nodes are in order a, D, B, C or a, C, B, D counterclockwise.
The specific steps of determining the arrangement sequence of the four nodes in the counterclockwise direction by using the vector product among the vectors comprise:
after the relative position relations of four near-field nodes P1, P2, P3 and P4 in the first plane of the boundary infinite unit are determined, two vectors are formed by connecting any three adjacent nodes in the four nodes end to end, and assuming that P1 and P3 and P2 and P4 are corner points of each otherTaking the point P1 as a starting point, the adjacent nodes are P2 and P4, the anticlockwise sequence of the four nodes is P1, P2, P3, P4 or P1, P4, P3 and P2, and a vector is calculated
And
cross product of
If it is
Normal vector to point P1 on the current boundary surface
When the included angle is an acute angle, namely:
the points P1, P2 and P3 are arranged in a counterclockwise direction, and the counterclockwise arrangement sequence of the four nodes is P1, P2, P3 and P4;
if it is
Normal vector to point P1 on the current boundary surface
When the included angle is an obtuse angle, namely:
the points P1, P2 and P3 are arranged clockwise, and the four nodes are arranged counterclockwise in the order of P1, P4, P3 and P2.
Further, the INP file (Job-4.INP) is opened in an ABAQUS model importing mode, and the specific steps of the ABAQUS that the Part three-dimensional infinite unit boundary is automatically generated comprise:
opening ABAQUS/CAE, opening an INP File (Job-4.INP) under a target folder through a Model Import mode (Import → Model) under a File menu, completing the modeling process of a boundary infinite unit, and checking the infinite element modeling effect under a specified Part.
Compared with the prior art, the invention has the beneficial effects that: the method mainly comprises the steps of utilizing a unit and a node definition method of an ABAQUS input file (.inp) according to a unit node definition rule in an ABAQUS three-dimensional infinite unit, completing automatic output of an infinite unit definition data line by certain Python programming, completing an input file of model definition according to a grammar rule of an INP file, and importing the ABAQUS/CAE to generate a boundary infinite unit. The method and the device have the advantages of avoiding the complicated process of manually modifying the INP file in the traditional method, having high automation degree, generating the infinite unit grid in a short time and greatly improving the modeling efficiency of the ABAQUS, along with simple operation.
Drawings
FIG. 1 is a flow chart of the technical solution of the present invention.
Figure 2 is an ABAQUS three-dimensional finite element model.
Fig. 3 is an infinite element far-field node generated using NCOPY.
FIG. 4 is a diagram of generating infinite element effects.
FIG. 5 is a model bottom surface bounding region infinite cell.
FIG. 6 is a model left boundary region infinite cell.
FIG. 7 is a model right border area infinite cell.
FIG. 8 is a model rear boundary region infinite element.
FIG. 9 is a model front edge boundary region infinite unit.
Detailed Description
The present invention will be described in further detail with reference to the accompanying drawings and specific embodiments.
As shown in fig. 1, the ABAQUS three-dimensional infinite element boundary fast modeling method based on the INP file in the embodiment of the present invention includes:
the method comprises the steps that a three-dimensional model is divided based on a three-dimensional unit grid, the rear central point of the three-dimensional model is located on the origin of a coordinate system, and the X axis, the Y axis and the Z axis of the coordinate system are the symmetry axes of the three-dimensional model;
101. establishing a finite element model, establishing a specified Part boundary node set as a near field node set of an infinite element, and exporting an ABAQUS input file (Job-1. inp);
establishing an ABAQUS/CAE three-dimensional finite element model as shown in FIG. 2, establishing a node set on a boundary surface of a designated Part as a near-field node (four nodes on a first surface of an infinite unit) set of a corresponding boundary infinite element by using a set tool under a Part module according to a research problem, wherein the node set conditions of different boundary areas are shown in Table 1; the analysis task Job-1 was created under the Job Module for the model of the problem and the ABAQUS Input file (Job-1.inp) was exported on Job Manager via Write Input.
102. Modifying the INP file to define a far-field node of an infinite unit by using a keyword (NCOPY) and storing the remote node as a new INP file (Job-2. INP);
modifying the INP file Job-1.INP, inserting a plurality of rows of node-defined keywords ([ NCOPY ]) in the specified Part definition line according to different boundary regions, and commanding as shown below
*Ncopy,Change Number＝2000,Old Set＝Node-Y1,New Set＝Node-Y2,Shift
0.0,-40.0,0.0
*Ncopy,Change Number＝4000,Old Set＝Node-X1,New Set＝Node-X3,Shift
-40.0,0.0,0.0
*Ncopy,Change Number＝6000,Old Set＝Node-X2,New Set＝Node-X4,Shift
40.0,0.0,0.0
*Ncopy,Change Number＝8000,Old Set＝Node-Z1,New Set＝Node-Z3,Shift
0.0,0.0,40.0
*Ncopy,Change Number＝10000,Old Set＝Node-Z2,New Set＝Node-Z4,Shift
0.0,0.0,-40.0
*Ncopy,Change Number＝12000,Old Set＝Node-X1Z1,New Set＝Node-X3Z3,Shift
-40.0,0.0,40.0
*Ncopy,Change Number＝14000,Old Set＝Node-X1Z2,New Set＝Node-X3Z4,Shift
-40.0,0.0,-40.0
*Ncopy,Change Number＝16000,Old Set＝Node-X2Z1,New Set＝Node-X4Z3,Shift
40.0,0.0,40.0
*Ncopy,Change Number＝18000,Old Set＝Node-X2Z2,New Set＝Node-X4Z4,Shift
40.0,0.0,-40.0
Copying the near field nodes by the specified offset distance by using the key word (NCOPY) to generate a far field node set with infinite elements at different zone boundaries as shown in Table 2, and storing the modified INP file as a new INP file (Job-2. INP).
The infinite element boundary far-field nodes are defined by copying and offsetting the near-field nodes for a certain distance, the node number of a new node is added with an integer value N on the basis of the original node number, one-to-one correspondence between the near-field nodes and the far-field nodes in the infinite element direction of the same infinite element is realized, the unit number difference N is obtained, the N value is selected in combination with the total number of nodes in the model, and the node number of the original finite element is ensured not to be repeated with the newly generated node number. The data line defines coordinate offset values of the newly created far-field node on the basis of the original near-field node.
TABLE 1 different boundary regions Infinite element near field and far field node sets
103, importing the modified INP file (Job-2.INP) by Abaqus/CAE, checking the generated infinite element far-field node and exporting a new INP file (Job-3. INP);
importing the modified INP File (Job-2.INP) in a File → Import → Model mode through a GUI (graphical user interface) of Abaqus/CAE, generating an infinite element far-field Node, under the condition of a Part module, clicking a Show Node display unit Node number under View → Part display Options → Mesh to View the generated infinite element far-field Node in different areas, as shown in FIG. 3, placing the imported Model in a Job module, creating a Job-3 task, and exporting a new INP File (Job-3.INP) through Write Input on JobManager.
Inserting a keyword line ([ ELEMENT ]) into a designated position of an INP file (Job-3.INP) to define an infinite unit, and storing the infinite unit as Job-4. INP;
the INP file (Job-3.INP) is edited according to the syntax rules of the INP file of ABAQUS, a new ELEMENT is defined by ELEMENT key lines and data lines, and the key line and data line insertion position defined by the ELEMENT must be located before the End-of-definition line End Part key of Part where the infinite ELEMENT boundary is located, and the far-field node set definition data line and the finite ELEMENT definition data line follow.
An INP file of ABAQUS mainly defines an infinite unit through an ELEMENT keyword, specifies the unit type as CIN3D8, and establishes an infinite boundary ELEMENT set on a corresponding boundary area; the data line is the unit number and the node number formed by the unit, the definition rule of the data line is given to the three-dimensional infinite unit ABAQUS help document, and the data line can also be read from other INP files containing unit definition data.
The above-described node number arrangement order defined by the data line cell satisfies the node order defined by the three-dimensional infinite cell (CIN3D8) in the ABAQUS help document.
The INP file of ABAQUS uses ELEMENT to perform infinite ELEMENT definition in two ways:
1) the data line defined by the infinite unit is directly inserted into the next line of the position of the infinite element definition key word of the corresponding area, and the command is as follows;
*Element,type＝CIN3D8,Elset＝bottomy
*Element,type＝CIN3D8,Elset＝leftx
*Element,type＝CIN3D8,Elset＝rightx
*Element,type＝CIN3D8,Elset＝frontz
*Element,type＝CIN3D8,Elset＝backz
*Element,type＝CIN3D8,Elset＝leftfrontcorner
*Element,type＝CIN3D8,Elset＝leftbackcorner
*Element,type＝CIN3D8,Elset＝rightfrontcorner
*Element,type＝CIN3D8,Elset＝rightbackcorner
*Element,type＝CIN3D8,Elset＝frontleftcorner
*Element,type＝CIN3D8,Elset＝frontrightcorner
*Element,type＝CIN3D8,Elset＝backleftcorner
*Element,type＝CIN3D8,Elset＝backrightcorner
2) inp, the content of which is simply the data line containing the current bounding area infinite unit definition that has previously completed the input-including the infinite unit number and the component node number, the command is as follows.
*Element,type＝CIN3D8,Elset＝bottomy,INPUT＝bottomy_element1.inp
*Element,type＝CIN3D8,Elset＝leftx,INPUT＝leftx_element1.inp
*Element,type＝CIN3D8,Elset＝rightx,INPUT＝rightx_element1.inp
*Element,type＝CIN3D8,Elset＝frontz,INPUT＝frontz_element1.inp
*Element,type＝CIN3D8,Elset＝backz,INPUT＝backz_element1.inp
*Element,type＝CIN3D8,Elset＝leftfrontcorner,INPUT＝leftfrontcorner_element.inp
*Element,type＝CIN3D8,Elset＝leftbackcorner,INPUT＝leftbackcorner_element.inp
*Element,type＝CIN3D8,Elset＝rightfrontcorner,INPUT＝rightfrontcorner_element.inp
*Element,type＝CIN3D8,Elset＝rightbackcorner,INPUT＝rightbackcorner_element.inp
*Element,type＝CIN3D8,Elset＝frontleftcorner,INPUT＝frontleftcorner_element.inp
*Element,type＝CIN3D8,Elset＝frontrightcorner,INPUT＝frontrightcorner_element.inp
*Element,type＝CIN3D8,Elset＝backleftcorner,INPUT＝backleftcorner_element.inp
*Element,type＝CIN3D8,Elset＝backrightcorner,INPUT＝backrightcorner_element.inp
Python programming constructs an infinite element boundary unit definition data line and inputs the infinite element boundary unit definition data line into an input file (Job-4.INP) of ABAQUS or a specified INP file, and the specific process is as follows:
1) reading a node number and a corresponding coordinate, a unit number and a component node number in an input file (Job-4.inp) of the ABAQUS by utilizing Python programming, and storing the node number and the corresponding coordinate, the unit number and the component node number in a specified list;
2) reading a key line number defined by an infinite unit in an INPUT file (Job-4.inp) of ABAQUS by utilizing Python programming and storing the key line number in a specified variable, or reading an INPUT parameter filename. inp written by an infinite unit definition data line;
3) traversing the node list of the finite element model according to the characteristics of the node coordinates, searching nodes on different boundaries according to the characteristics of the coordinate values of the nodes of the boundaries, and adding the nodes to the specified boundary node list;
4) searching boundary units by traversing the unit list of the finite element model according to the relationship between the unit composition node coordinates and the characteristics of the node coordinates on the boundary, and adding the boundary units to the specified boundary unit list;
5) traversing the appointed boundary node list, taking out any four nodes A, B, C and D, and judging whether the four nodes are four nodes on the first surface of the boundary infinite unit near field;
6) if the four nodes A, B, C and D are four nodes on the first surface of the boundary infinite unit near field, solving a vector included angle relation according to the quantity product of the vectors to determine the relative position relation of the four nodes;
7) determining the arrangement sequence of the four nodes in the counterclockwise direction as Q1, Q2, Q3 and Q4 by using the vector product among the vectors;
8) the infinite unit serial number is determined by a Part unit number a specified in the finite model, a defined boundary infinite unit number b and an infinite unit definition sequence c in the region, and then the current infinite unit number is Q ═ a + b + c;
9) given a data line output specifying a boundary cell infinite element definition:
Q,Q1,Q2,Q3,Q4,Q1+N,Q2+N,Q3+N,Q4+N
wherein: q is an infinite element number, Q1, Q2, Q3, Q4 are four near-field nodes, Q1+ N, Q2+ N, Q3+ N, and Q4+ N are four far-field nodes;
10) two infinite unit definition data line output modes, wherein the former mainly adopts a key line ① and a data line ① aiming at infinite unit definition, namely the unit definition data line is directly inserted into the next line of the key definition position in Job-4.inp and is stored;
the latter mainly adopts a key line ② and a data line ② for the infinite unit definition, writes the data line of the unit definition into an INPUT parameter file.
106. The INP file (Job-4.INP) is opened in a mode of importing the ABAQUS model, and the ABAQUS designates that Part three-dimensional infinite unit boundaries are automatically generated.
Opening ABAQUS/CAE, opening an INP File (Job-4.INP) under a target folder through a Model Import mode (Import → Model) under a File menu, completing a modeling process of a boundary infinite unit, and viewing an infinite element modeling effect under a designated Part, as shown in FIG. 4. Fig. 5-9 are diagrams of infinite elements of the generation of different bounding regions.
Claims (10)
1. An ABAQUS three-dimensional infinite element boundary rapid modeling method based on an INP file is characterized in that according to an ABAQUS three-dimensional infinite element node definition rule, an ABAQUS input file is utilized, an INP unit and node definition method is utilized, automatic output of ABAQUS infinite element definition data lines is realized by means of Python programming, an input file of model definition is completed according to a grammar rule of the INP file, and an ABAQUS/CAE generation boundary infinite element is imported; the method comprises the following specific steps:
establishing a finite element model, establishing a specified Part boundary node set as a near field node set of an infinite element, and exporting the ABAQUS input file Job-1. inp;
modifying the INP file, defining a far-field node of an infinite unit by using a keyword NCOPY, and storing the remote node as a new INP file Job-2. INP;
the key line and data line insertion position defined by the far-field node must be positioned before the definition End line (End Part) key word of Part where the infinite element boundary is positioned, and behind the definition data line of the near-field node set;
leading in the modified INP file Job-2.INP by the ABAQUS/CAE, checking the generated infinite element far-field node and leading out a new INP file Job-3. INP;
inserting a keyword line ELEMENTS into the designated position of the INP file Job-3.INP to define an infinite unit, and storing the infinite unit as Job-4. INP;
the specified position is positioned before a definition End row (End Part key word) of Part where the infinite element boundary is positioned, and the far field node set definition data row and the finite element unit definition data row are positioned behind;
python programming constructs an infinite element boundary unit definition data line and inputs the infinite element boundary unit definition data line into an input file Job-4.INP of ABAQUS or a specified INP file;
and opening the designated INP file or Job-4.INP in an ABAQUS model importing mode, wherein ABAQUS designates Part three-dimensional infinite unit boundaries to be automatically generated.
2. The ABAQUS three-dimensional infinite element boundary rapid modeling method based on the INP file as claimed in claim 1,
establishing an infinite element near-field node set in a finite element model and deriving an ABAQUS input file Job-1.inp comprises the following steps:
establishing an ABAQUS/CAE three-dimensional finite element model, and establishing a node set on a boundary surface of a designated Part as a near-field node set of a corresponding boundary infinite element by using a set tool under a Part module according to a research problem, namely four nodes on a first surface of the infinite element;
establishing an analysis task Job-1 for the model of the research problem under a Job module, and exporting an ABAQUS Input file Job-1.inp on a Job Manager through Write Input;
modifying the INP file, generating a far-field node of an infinite unit by using a keyword NCOPY, and additionally storing as a new INP file Job-2. INP:
modifying an INP file Job-1.INP, and inserting a plurality of lines of keywords NCOPY defined by nodes in a specified Part definition line according to different boundary regions;
forming a far-field node of infinite elements of different zone boundaries by using a keyword NCOPY;
saving the modified INP file as a new INP file Job-2. INP;
importing the modified INP file Job-2.INP by ABAQUS/CAE, checking the generated infinite element far-field node and deriving a new INP file Job-3.INP comprises:
importing the modified INP File Job-2.INP in a way of File → Import → Model through a graphical user interface GUI of ABAQUS/CAE, and generating a far-field node of an infinite element, but temporarily not displaying the node;
under the condition of a Part module, checking generated infinite element far-field nodes in different areas by clicking a Show node labels of Show node labels under View → Part Display Options → Mesh;
importing a model into a Job module, creating a Job-3 task, and exporting a new INP file Job-3.INP through a Write Input on a Job Manager;
the INP file Job-3.INP specifies the position to insert the keyword line ELEMENTS to define an infinite unit, and further includes for Job-4. INP:
editing an INP file Job-3.INP, and inserting a keyword line ELEMENT in a designated line to define an infinite unit;
and the INP file inserted with the ELEMENT keyword line and the data line is saved as a new INP file Job-4. INP.
3. The method for rapidly modeling the ABAQUS three-dimensional infinite element boundary based on the INP file as claimed in claim 2, wherein the generating the far-field nodes of the infinite elements of the boundary of different areas using the keyword NCOPY comprises:
the key word lines and data lines defined by the nodes must be edited according to the grammar rules of the INP file of ABAQUS;
new nodes are defined by NCOPY key rows and data rows.
4. The method for rapidly modeling ABAQUS three-dimensional infinite element boundary based on the INP file as claimed in claim 3, wherein the keyword line and the data line must be edited according to the grammar rule of the INP file of ABAQUS comprises:
1) the far-field node defines a Keyword Line as follows:
*NCOPY,CHANGE NUMBER＝N,OLD SET＝near_field_NodeSetName,NEW SET＝far_field_NodeSetName,SHIFT
2) the far-field node defines a Data Line as:
Shifting-x,Shifting-y,Shifting-z
the key line and data line inserting positions defined by the nodes are necessarily positioned in front of a definition ending line (End Part) key word of Part where an infinite element boundary is positioned, and behind the definition data lines of the near-field node set;
defining a new node by the NCOPY key line and the data line comprises:
copying an offset designated distance through a near field node, defining an infinite element boundary far field node, and adding an integer value N to the node number of a new node on the basis of the original node number;
the near-field nodes and far-field nodes in the infinite element direction of the same infinite unit are in one-to-one correspondence, and the unit numbers have a difference of N;
the data line defines coordinate offset values of the newly created far-field node on the basis of the original near-field node.
5. The method for modeling ABAQUS three-dimensional infinite ELEMENT boundary fast based on the INP file as claimed in claim 2, wherein editing the INP file Job-3.INP and inserting a keyword x ELEMENT row at a designated position for infinite ELEMENT definition comprises:
defining an infinite cell by an ELEMENT key row and a data row;
the key word lines and data lines defined by the infinite unit must be edited according to the grammar rules of the INP file of ABAQUS;
the key line and data line insertion position of the node definition must be before the End-of-definition line End Part key of Part where the infinite element boundary is located, and the far-field node set definition data line and finite element definition data line are after.
6. The method for rapidly modeling ABAQUS three-dimensional infinite ELEMENT boundaries based on the INP file as set forth in claim 3, wherein defining the boundary infinite ELEMENT by the ELEMENT key line and the data line comprises:
the definition of the ABAQUS unit and the node is that a geometrical shape is created and a unit grid is divided through a preprocessor ABAQUS/CAE to form a unit node, wherein the ABAQUS infinite unit is defined in an INP file by manually editing the INP file, inserting an ELEMENT keyword, assigning a unit number to the infinite unit, defining the unit through the designated unit node number and grouping boundary infinite ELEMENTs at the same time;
considering that the unit number allocated on the ASSEMBLY asset is not unique and needs to be distinguished in combination with Part, and the unit number allocated on the Part is unique, the definition of the boundary infinite element is only defined in the designated Part;
defining an infinite unit through an ELEMENT keyword, designating the unit type as CIN3D8, and establishing an infinite boundary ELEMENT set on a corresponding boundary area;
the data line defined by the infinite unit is a unit number and a node number formed by the units;
ABAQUS infinite cell defined data lines or read from other INP files containing cell definition data;
the node number arrangement order defined by the data line units meets the node order defined by a three-dimensional infinite unit CIN3D8 in the ABAQUS help document;
the key line and data line defined by the infinite unit must be edited according to the syntax rules of the INP file of ABAQUS, including:
1) the keyword line defined by the infinite unit of the infinite element boundary has two modes, which are respectively:
①*Element,type＝CIN3D8,Elset＝Infinite_Element_SetName
②*Element,type＝CIN3D8,Elset＝Infinite_Element_SetName,INPUT＝filename.inp
2) the corresponding infinite unit definition data line DataLine respectively corresponds to the key line in two ways:
① the data line defined by the infinite element is directly inserted into the next line of the position of the infinite element definition key of the corresponding area, which comprises an infinite element number and a component node number, namely:
Infinite_element_Num,NodeP1,NodeP2,NodeP3,NodeP4,NodeP5,NodeP6,NodeP7,NodeP8
② the line of data defined by an infinite cell is given by a file. inp file whose contents are simply the line of data defined by the infinite cell of the current bounding area containing the pre-completed input-including the infinite cell number and the constituent node number, i.e.:
Infinite_element_Num,NodeP1,NodeP2,NodeP3,NodeP4,NodeP5,NodeP6,NodeP7,NodeP8。
7. the method for modeling ABAQUS three-dimensional Infinite element boundary fast based on INP file according to claim 6, wherein the data line Infinite _ element _ Num, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8 defined by Infinite elements comprises:
the node numbers of the four far-field nodes are larger than the node numbers of the near-field nodes on the corresponding infinite-direction unit edges, namely the nodes on the finite-element boundary, by N, namely:
according to the infinite unit definition rule, four nodes NodeP1, NodeP2, NodeP3 and NodeP4 in the near field of the first surface of the infinite unit are required to be arranged in a sequence of the four nodes in the near field in a counterclockwise direction when the four nodes are observed from the far field to the near field of the infinite unit;
the unit number designated by the infinite unit definition is determined by the number of finite units on the current Part, the number of infinite units in the defined boundary area and the order of the infinite unit definition in the area.
8. The ABAQUS three-dimensional infinite element boundary rapid modeling method based on the INP file as claimed in claim 7, wherein the step of constructing the infinite element boundary unit definition data row by using Python programming and inputting the infinite element boundary unit definition data row into the input file Job-4.INP of the ABAQUS or the designated INP file comprises the following steps:
1) reading a node number and a corresponding coordinate, a unit number and a component node number in an input file Job-4.inp of the ABAQUS by utilizing Python programming, and storing the node number and the corresponding coordinate, the unit number and the component node number in a specified list;
2) reading the key word line number defined by an infinite unit in an INPUT file Job-4.INP of ABAQUS by Python programming and storing the key word line number in a specified variable, or reading an INPUT parameter written in the infinite unit definition data line-the INP file.
3) Traversing the node list of the finite element model according to the characteristics of the node coordinates, searching nodes on different boundaries according to the characteristics of the coordinate values of the nodes of the boundaries, and adding the nodes to the specified boundary node list;
4) searching a boundary unit by traversing a unit list of the finite element model according to the relationship between the unit composition node coordinates and the characteristics of the node coordinates on the boundary, and adding the boundary unit to an appointed boundary unit list;
5) traversing the appointed boundary node list, taking out any four nodes A, B, C and D, and judging whether the four nodes are four nodes on the first surface of the boundary infinite unit near field;
6) if the A, B, C and D nodes are four nodes on the first surface of the boundary infinite unit near field, solving a vector included angle relation according to the quantity product of the vectors to determine the relative position relation of the four nodes;
7) determining the arrangement sequence of the four nodes in the counterclockwise direction as Q1, Q2, Q3 and Q4 by using the vector product among the vectors;
8) the infinite unit serial number is determined by a Part unit number a specified in the finite model, a defined boundary infinite unit number b and an infinite unit definition sequence c in the region, and then the current infinite unit number is Q ═ a + b + c;
9) given a data line output specifying a boundary cell infinite element definition:
Q,Q1,Q2,Q3,Q4,Q1+N,Q2+N,Q3+N,Q4+N
wherein: q is an infinite element number, Q1, Q2, Q3, Q4 are four near-field nodes, Q1+ N, Q2+ N, Q3+ N, and Q4+ N are four far-field nodes;
10) two infinite unit definition data line output modes, wherein the former adopts a key line ① and a data line ① aiming at infinite unit definition, namely the unit definition data line is directly inserted into the next line of the key definition position in Job-4.inp and is stored;
the latter adopts key word line ② and data line ② for the infinite unit definition, writes the data line of the unit definition into the INPUT parameter file. inp file in the infinite unit definition line, and ABAQUS automatically reads the data line in the file.
9. The ABAQUS three-dimensional infinite element boundary rapid modeling method based on the INP file as claimed in claim 8, wherein traversing the designated boundary node list and retrieving any four nodes therein, and determining whether the node is four nodes on the first near-field surface of the infinite element model comprises:
by utilizing the member test function of Python, if four nodes taken out from the boundary node list are four of the boundary unit composition nodes, the four nodes are four near-field nodes on the first surface of the boundary infinite unit;
if A, B, C and D four nodes are four nodes on the first surface of the boundary infinite unit near field, solving two vector included angles according to the vector quantity product to determine the relative position relationship of the four nodes comprises the following steps:
with point a as the first point of the quadrilateral, the sizes of ∠ BAC, <tttransition = & <t/t >tbad and ∠ CAD are respectively calculated using the vector quantity product and summed:
let SUM ∠ BAC + ∠ BAD + ∠ CAD:
1) if SUM is 2 ∠ BAC, point a and point D, point B and point C are diagonal nodes, and the counterclockwise direction of the nodes is A, B, D, C or A, C, D, B;
2) if SUM is 2 ∠ BAD, point a and point C, point B and point D are diagonal nodes to each other, and the counterclockwise direction sequence of the nodes is A, B, C, D or A, D, C, B;
3) if SUM is 2 ∠ CAD, point a and point B, point C and point D are diagonal nodes to each other, and the counterclockwise direction sequence of the nodes is A, D, B, C or A, C, B, D;
determining the counterclockwise arrangement order of the four nodes using the vector product between the vectors includes:
after the relative position relations of four near-field nodes P1, P2, P3 and P4 in a first plane of a boundary infinite unit are determined, two vectors are formed by connecting any three adjacent nodes in the four nodes end to end, if the P1 and the P3, and the P2 and the P4 are mutually corner points, the P1 point is taken as a starting point, the adjacent nodes are necessarily P2 and P4, the counterclockwise sequence of the four nodes is P1, P2, P3 and P4, or P1, P4, P3 and P2, and the vectors are calculated
And
cross product of
If it is
Normal vector to point P1 on the current boundary surface
When the included angle is an acute angle, namely:
the points P1, P2 and P3 are arranged in a counterclockwise direction, and the counterclockwise arrangement sequence of the four nodes is P1, P2, P3 and P4;
if it is
Normal vector to point P1 on the current boundary surface
When the included angle is an obtuse angle, namely:
the points P1, P2 and P3 are arranged clockwise, and the four nodes are arranged counterclockwise in the order of P1, P4, P3 and P2.
10. The method for rapidly modeling ABAQUS three-dimensional infinite element boundary based on the INP file as claimed in claim 7, wherein the step of opening the INP file or Job-4.INP by means of ABAQUS model import, wherein ABAQUS specifies that Part three-dimensional infinite element boundary is automatically generated comprises the steps of:
opening ABAQUS/CAE, opening an INP File Job-4.INP under a target folder through a Model Import mode Import → Model under a File menu, completing a modeling process of a boundary infinite unit, and checking an infinite element modeling effect under a specified Part.
Priority Applications (1)
| Application Number | Priority Date | Filing Date | Title |
|---|---|---|---|
| CN201710270976.4A CN107145651B (en) | 2017-04-24 | 2017-04-24 | ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file |
Applications Claiming Priority (1)
| Application Number | Priority Date | Filing Date | Title |
|---|---|---|---|
| CN201710270976.4A CN107145651B (en) | 2017-04-24 | 2017-04-24 | ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file |
Publications (2)
| Publication Number | Publication Date |
|---|---|
| CN107145651A CN107145651A (en) | 2017-09-08 |
| CN107145651B true CN107145651B (en) | 2020-04-28 |
Family
ID=59774761
Family Applications (1)
| Application Number | Title | Priority Date | Filing Date |
|---|---|---|---|
| CN201710270976.4A Expired - Fee Related CN107145651B (en) | 2017-04-24 | 2017-04-24 | ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file |
Country Status (1)
| Country | Link |
|---|---|
| CN (1) | CN107145651B (en) |
Families Citing this family (5)
| Publication number | Priority date | Publication date | Assignee | Title |
|---|---|---|---|---|
| CN107679341B (en) * | 2017-10-30 | 2021-03-02 | 南京理工大学 | Finite element parametric modeling method for barrel structure |
| CN109446734B (en) * | 2018-12-17 | 2022-09-27 | 西安建筑科技大学 | Method for adding spring unit in steel pipe concrete finite element model |
| CN111046608B (en) * | 2019-12-19 | 2023-07-18 | 东南大学 | Basalt fiber asphalt cement finite element model modeling method |
| CN111209694B (en) * | 2019-12-30 | 2023-12-15 | 北京工业大学 | Structure identification method for rigidity and axial force of truss structure |
| CN111159951B (en) * | 2019-12-31 | 2023-08-18 | 哈尔滨工业大学（深圳） | Coupling method based on ABAQUS finite element and boundary element |
Citations (2)
| Publication number | Priority date | Publication date | Assignee | Title |
|---|---|---|---|---|
| DE102004039982A1 (en) * | 2004-08-12 | 2006-02-23 | Basf Ag | Microstructure-based modeling of mechanical characteristics of block copolymer comprises generating hypothetical morphologies and cross-linking finite elements, producing several domains and simulating deformation of cross-link of elements |
| CN104361631A (en) * | 2014-10-24 | 2015-02-18 | 哈尔滨工业大学 | Method for building vibration response three-dimensional numerical models of railway roadbeds in seasonally frozen ground regions in parameterized manner |
-
2017
- 2017-04-24 CN CN201710270976.4A patent/CN107145651B/en not_active Expired - Fee Related
Patent Citations (2)
| Publication number | Priority date | Publication date | Assignee | Title |
|---|---|---|---|---|
| DE102004039982A1 (en) * | 2004-08-12 | 2006-02-23 | Basf Ag | Microstructure-based modeling of mechanical characteristics of block copolymer comprises generating hypothetical morphologies and cross-linking finite elements, producing several domains and simulating deformation of cross-link of elements |
| CN104361631A (en) * | 2014-10-24 | 2015-02-18 | 哈尔滨工业大学 | Method for building vibration response three-dimensional numerical models of railway roadbeds in seasonally frozen ground regions in parameterized manner |
Non-Patent Citations (2)
| Title |
|---|
| 山区特殊地质条件下地基-箱基-上部结构地震响应分析;尚军;《天津城建大学学报》;20140831;第20卷(第3期);全文 * |
| 背后空洞引起高速铁路隧道衬砌裂缝形态的FEM对比分析;雷波等;《铁道标准设计》;20150930;第59卷(第9期);全文 * |
Also Published As
| Publication number | Publication date |
|---|---|
| CN107145651A (en) | 2017-09-08 |
Similar Documents
| Publication | Publication Date | Title |
|---|---|---|
| CN107145651B (en) | ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file | |
| CN109359351B (en) | Three-dimensional modeling method for pipeline and pipeline design method | |
| CN110765523A (en) | BIM technology-based rapid construction method for deep foundation pit support structure | |
| Seiler et al. | Robust interactive cutting based on an adaptive octree simulation mesh | |
| CN105718643A (en) | Optimization view angle based ship production design drawing-inspection device implementation method | |
| CN110569580B (en) | Urban street space vitality simulation method, system, computer equipment and medium | |
| CN109858161A (en) | A kind of Abaqus Meshing Method based on Midas modeling and Matlab conversion | |
| Nan | Easy3D: a lightweight, easy-to-use, and efficient C++ library for processing and rendering 3D data | |
| CN113486429A (en) | Automatic construction method of space intersection structure based on interpolation algorithm | |
| CN116630589A (en) | Data linkage editing method and device between three-dimensional virtual scene and two-dimensional view | |
| CN114638131B (en) | Crystal plasticity finite element modeling method based on electron back scattering diffraction analysis and Gmesh software | |
| Altabtabai et al. | A user interface for parametric architectural design reviews | |
| CN113220199A (en) | Method for assisting in establishing finite element model | |
| US9141734B2 (en) | System and method of refining a topological indexed mesh | |
| JP2001099880A (en) | Electromagnetic field analyzing method and record medium recording analytical program | |
| CN113378427A (en) | Calculation method for evaluating wind load fracture resistance of branches and trunks of arbor | |
| Gaither et al. | The National Grid Project: a system overview | |
| JP2817917B2 (en) | Solid CAD system | |
| Goanță | Comparative study of" revolve" command in the average-class design software taught in the higher education | |
| Liu et al. | Geometry pretreatment method for the 3D modular characteristic method based on AutoCAD | |
| Zhang | Research on 3D Variable Design of Corrugated Box Based on SolidWorks | |
| Yanjie et al. | UG-based research and development of 3D pipe layout system of the aircraft engine | |
| LU504992B1 (en) | Method and apparatus for establishing three-dimensional (3d) geological environment evaluation model for underground space, and device | |
| CN109684675B (en) | Method for analyzing strength of aviation thin-wall support based on abaqus plate coupling | |
| Jones | The development of problem solving environments for computational engineering |
Legal Events
| Date | Code | Title | Description |
|---|---|---|---|
| PB01 | Publication | ||
| PB01 | Publication | ||
| SE01 | Entry into force of request for substantive examination | ||
| SE01 | Entry into force of request for substantive examination | ||
| GR01 | Patent grant | ||
| GR01 | Patent grant | ||
| CF01 | Termination of patent right due to non-payment of annual fee |
Granted publication date: 20200428 Termination date: 20210424 |
|
| CF01 | Termination of patent right due to non-payment of annual fee |