CN107145651A - The three-dimensional infinite element border fast modeling methods of ABAQUS based on INP files - Google Patents

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 element boundary modeling. According to the theory of infinite element definition, the method for defining nodes and elements in the ABAQUS input file .inp is used. Based on the Python programming technology, the data line defined by the infinite element is output, and the input file is generated and imported into ABAQUS/CAE according to the syntax rules of the INP file, so as to realize the automatic generation of the infinite element boundary of ABAQUS. The invention is simple to operate, can generate an ABAQUS infinite element boundary model in a short time, and greatly improves the ABAQUS modeling speed.

Description

ABAQUS 3D Infinite Element Boundary Rapid Modeling Method Based on INP File

technical field

The invention relates to an infinite element boundary modeling method, in particular to an ABAQUS three-dimensional infinite element boundary rapid modeling method based on an INP file.

Background technique

The emergence and rapid development of computers provide powerful tools for engineering analysis, making it possible to use numerical simulation to solve many large-scale engineering practical problems. As the most commonly used numerical simulation method, the finite element method is widely used in geotechnical, structural, earthquake and water conservancy engineering fields. The problem faced by the finite element method is how to use a "finite" model to simulate the actual "infinite" area. The common solution is to ignore the influence of the "infinite" area boundary according to Saint-Venant's principle, and use the truncated boundary to take "enough" The size of the model is divided into finite element meshes of the geometric size, and the corresponding approximate constraint boundary conditions are imposed on the artificial boundaries. In actual calculation, it is difficult to identify the size of this "large enough" model. The calculation cost is low when the area is small, but the accuracy of the result is poor; when the area is large, it meets certain accuracy requirements, but the calculation cost is high. Especially for wave calculation problems, the finite element calculation results are often distorted due to the reflection and scattering of waves on the grid boundary.

By introducing boundary elements to establish a reasonable artificial boundary, the reflection of the finite element boundary caused by artificial truncation on the boundary of various fluctuations in the foundation can be minimized, thereby greatly reducing the number of elements and improving calculation efficiency. Common artificial boundaries such as viscous boundaries, paraxial approximation boundaries, transmission boundaries, viscoelastic boundaries, infinite element boundaries, etc.

As a way of simulating infinite regions, the emergence of infinite elements provides an important way to overcome the defects of finite element calculation methods and solve the problems of infinite region boundary simulation. Conceptually, the infinite element belongs to the extension of the finite element. Its main idea is to define the physical field of the infinite domain through the geometrically infinite "finite" unit. And because the infinite element must reflect the boundary characteristics of the near field or combine with the finite element that simulates the near field, it actually only tends to infinity in one direction, so it is also called a semi-infinite element. From the concept of generalized finite element, infinite element still belongs to the category of finite element. In short, the infinite element is proposed to overcome the finite element when solving the unbounded domain problem. It is often used together with the conventional finite element to solve more complex unbounded problems. It is a supplement to the finite element method, so its "coordination" with the finite element method "Inherent, it has more advantages than boundary elements and other numerical methods for solving unbounded domain problems.

A lot of experience in solving infinite domain problems shows that the coupling model of finite element and infinite element has wide practicability in solving practical engineering problems. Especially in the study of internal fluctuations, such as train vibration and blasting, and the seismic dynamics of external vibrations, infinite elements have shown obvious advantages in simulating and approximately simulating infinite domain problems. In addition, the finite element and infinite element coupling models are also widely used in the fields of electromagnetism, thermodynamics, and acoustics, and have achieved good simulation results. The large-scale finite element calculation software ABAQUS and ANSYS have improved a variety of infinite element types to simulate the infinite domain problem of finite element calculation. Among them, ABAQUS is widely used in dynamic calculation in the field of geotechnical engineering because of its powerful dynamic nonlinear calculation ability.

ABAQUS provides first-order and second-order infinite elements, including plane strain, plane stress, axisymmetric and three-dimensional infinite element elements, which are developed based on static calculation analysis such as Zienkiewicz and dynamic response analysis such as Lysmer, which can be used for static Infinite domain problem solving, and as an infinite element dynamic artificial boundary to solve the local source vibration problem in the domain, that is, it is effective for the simulation of the outward traveling wave that passes through the artificial boundary from the finite domain and enters the infinite domain, while the external source incident problem is performed on the basis of ABAQUS infinite elements Secondary development has also successfully solved the problem of earthquake dynamics. The common three-dimensional infinite elements of ABAQUS infinite element dynamic artificial boundary include CIN3D8, CIN3D12R ^(S) and CIN3D18R (S), etc. This element can be combined with standard finite elements to simulate the near field area with finite elements and the far field with infinite elements area.

Although ABAQUS boundary infinite element provides convenience for static infinite element and dynamic artificial boundary simulation. However, because the node numbers in the infinite element must ensure that the first surface of the element is the interface between the finite element and the infinite element, so as to ensure the directionality of the infinite element element, the extension direction of the element is from the near field to the far field area. Infinite elements cannot be directly defined in ABAQUS, only the boundary part of the infinite element can be built by default during modeling, and other element types are used to distinguish, exported to the ABAQUS input file (.inp), and then compared with the model to manually modify the ABAQUS input file (.inp) element node order for infinite element boundaries. Especially for three-dimensional boundary infinite elements, the modification process is cumbersome, especially when the analysis task is large, it will consume more manpower and time, and there are often cases of manual operation errors resulting in grid operation errors.

Invention content:

The technical problem to be solved by the present invention is to provide a fast modeling method of ABAQUS three-dimensional infinite element boundary based on the INP file, which overcomes the cumbersome modeling process and low modeling efficiency of the existing boundary infinite element model of ABAQUS, considering the characteristics of ABAQUS infinite element and The characteristics of ABAQUS's input INP file model definition are simple to operate and highly automated. It can generate infinite element meshes in a short period of time, which greatly improves the modeling efficiency of ABAQUS.

In order to solve the problems of the technologies described above, the technical solution adopted in the present invention is:

According to the definition rules of unit nodes in ABAQUS three-dimensional infinite element (3D infinite element), use the unit and node definition method of ABAQUS input file (. The rules complete the input file of the model definition and import it into ABAQUS/CAE to generate boundary infinite elements.

The technical solution adopted by the present invention to solve its technical problems comprises the following steps:

Establish the finite element model and create the specified Part boundary node set as the near-field node set of the infinite element, and export the ABAQUS input file (Job-1.inp);

Modify the INP file and use the keyword (*NCOPY) to define the far-field nodes of the infinite element, and save it as a new INP file (Job-2.inp);

Abaqus/CAE imports the modified INP file (Job-2.inp), checks the generated infinite element far-field nodes and exports the new INP file (Job-3.inp);

INP file (Job-3.inp) inserts the keyword line (*ELEMENT) at the specified position to define the infinite element, and save it as Job-4.inp;

Python programming constructs the infinite element boundary cell definition data line and inputs it to the ABAQUS input file (Job-4.inp) or the specified INP file;

Open the above INP file (Job-4.inp) by importing the ABAQUS model, and the ABAQUS specified Part 3D infinite element boundary is automatically generated.

Further, the specific steps of establishing the infinite element near-field node set in the finite element model and exporting the ABAQUS input file (Job-1.inp) include:

Establish the ABAQUS/CAE three-dimensional finite element model, use the set tool under the Part module to establish the node set on the boundary surface of the specified Part as the near-field node set corresponding to the boundary infinite element, that is, the four nodes on the first surface of the infinite element nodes;

Create an analysis task Job-1 for the model of the above problem under the Job module, and export the ABAQUS input file (Job-1.inp) through Write Input on the Job Manager.

Modify the above INP file and use the keyword (*NCOPY) to generate the far-field node of the infinite unit, and save it as a new INP file (Job-2.inp). The main contents include:

Modify the above INP file Job-1.inp, insert multi-line node definition keywords (*NCOPY) in the specified Part definition line according to different boundary areas;

Use the keyword (*NCOPY) to copy and offset the near-field nodes to generate far-field nodes of infinite elements in different regions;

Save the above modified INP file as a new INP file (Job-2.inp);

Abaqus/CAE imports the modified INP file Job-2.inp, checks the generated infinite element far-field nodes and exports the new INP file Job-3.inp including:

Import the modified INP file Job-2.inp through the Abaqus/CAE graphical user interface GUI in the form of File→Import→Model, and the far-field nodes of the infinite element are generated, but they cannot be displayed temporarily;

Under the condition of the Part module, click Show NodeLabels under View→Part Display Options→Mesh to display the unit node number, and view the generated infinite element far-field nodes in different regions;

Put the imported model in the Job module, create a new Job-3 task, and export a new INP file Job-3.inp through WriteInput on the Job Manager;

The INP file Job-3.inp inserts the keyword line *ELEMENT to define the infinite element at the specified position, and save it as Job-4.inp including:

Edit the INP file Job-3.inp, insert the keyword line *ELEMENT in the specified line to define the infinite element;

The INP file after inserting the *ELEMENT keyword row and the data row is saved as a new INP file Job-4.inp.

Further, use the keyword (*NCOPY) to copy and offset the near-field nodes to generate the far-field nodes of different boundary infinite elements. The main contents include:

The keyword line and data line defined by the node must be edited according to the syntax rules of the INP file of ABAQUS;

New nodes are defined via the *NCOPY keyword line and the data line.

Further, the keyword line and data line must be edited according to the grammar rules of the ABAQUS INP file. The main content refers to:

1) The far-field node defines the Keyword Line as:

*NCOPY,CHANGE NUMBER=N,OLD SET=near_field_NodeSetName,NEW SET=far_field_NodeSetName,SHIFT

2) The far-field node defines the Data Line as:

Shifting-x, Shifting-y, Shifting-z

The insertion position of the key line and data line defined by the above nodes must be before the definition end line *End Part keyword of the Part where the infinite element boundary is located, and after the data line defined by the near-field node set.

Defining new nodes through *NCOPY keyword lines and data lines mainly refers to:

By copying the near-field node and offsetting a certain distance, define the far-field node of the infinite element boundary, and the node number of the new node is increased by the integer value N on the basis of the original node number;

One-to-one correspondence between near-field nodes and far-field nodes along the infinite element direction of the same infinite element is realized, and the element numbers differ by N;

The data line defines the coordinate offset value of the newly created far-field node based on the original near-field node.

Further, edit the INP file (Job-3.inp), insert the keyword (*ELEMENT) line at the specified position to define the infinite element. The details refer to:

Define new infinite elements via *ELEMENT keyword row and data row;

The keyword line and data line defined by the infinite unit must be edited according to the syntax rules of the INP file of ABAQUS;

The keyword row and data row insertion position of the above unit definition must be before the definition end row *End Part keyword of the Part where the infinite element boundary is located, and after the far field node set definition data row and the finite element unit definition data row.

Furthermore, the specific content of defining boundary infinite elements through *ELEMENT keyword line and data line includes:

The definition of ABAQUS units and nodes is mainly through its pre-processor ABAQUS/CAE, creating geometric shapes and dividing unit grids to form unit nodes. The ABAQUS infinite units here are defined in the INP file by manually editing the INP file and inserting * The ELEMENT keyword assigns an element number to the infinite element, and defines the element by specifying the element node number, and can group the boundary infinite elements.

Considering that the unit number assigned on the assembly (ASSEMBLY) is not unique, it needs to be distinguished in combination with the part (Part), and the unit number assigned on the part is unique, so the definition of the boundary infinite element is only defined in the specified Part;

Mainly define the infinite element through the *ELEMENT keyword, specify the element type as CIN3D8, and establish an infinite boundary element set on the corresponding boundary area;

The data line defined by the infinite unit is the specified unit number and the node number composed of the unit;

Data lines defined by ABAQUS infinite elements can also be read from other INP files containing element definition data;

The arrangement order of the node numbers defined by the above-mentioned data line unit meets the order of the nodes defined by the three-dimensional infinite unit (CIN3D8) in the ABAQUS help document.

The keyword line and data line defined by the infinite unit must be edited according to the grammatical rules of the INP file of ABAQUS. Specifically, it refers to:

1) There are two ways to define the Keyword Line (Keyword Line) of the infinite element boundary, which are:

①*Element, type=CIN3D8, Elset=Infinite_Element_SetName

②*Element, type=CIN3D8, Elset=Infinite_Element_SetName, INPUT=filename.inp

2) The corresponding infinite cell definition data line (Data Line) can be defined in two ways, respectively corresponding to the above key line:

①The data line defined by the infinite element is directly inserted into the next line where the keyword of the infinite element definition in the corresponding area is located, mainly including the infinite element number and the component node number, namely:

Infinite_element_Num, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8

②The data line defined by the infinite unit is given by filename.inp, and the content of this file only includes the data line defined by the infinite unit in the current boundary area that has been input in advance—including the infinite unit number and the component node number, namely:

Infinite_element_Num, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8.

Further, the data rows Infinite_element_Num, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8 related conventions defined by the infinite element include:

According to claims 5 and 6, the node numbers of the four nodes in the far field are larger than the node number values of the near-field nodes (nodes on the finite element boundary) on the edge of the corresponding element along the infinite direction, that is:

According to the definition rules of the infinite element, the four nodes NodeP1, NodeP2, NodeP3 and NodeP4 in the near field of the first surface of the infinite element must meet the order of the four nodes in the near field in the counterclockwise direction when observing from the far field to the near field of the infinite element;

The unit number specified 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 infinite unit definitions in the area.

Further, using Python programming to construct the infinite element boundary cell definition data line and input it to the input file (Job-4.inp) of ABAQUS or the specified INP file specifically includes the following steps:

1) Use Python programming to read the node numbers and corresponding coordinates, unit numbers and component node numbers in the ABAQUS input file (Job-4.inp), and store them in the specified list;

2) Use Python programming to read the keyword line number defined by the infinite unit in the input file (Job-4.inp) of ABAQUS and store it in the specified variable, or read the INPUT parameter written by the infinite unit definition data line—ABAQUS The read INP file filename.inp;

3) Traversing the node list of the above-mentioned finite element model according to the characteristics of node coordinates, searching for nodes on different boundaries according to the characteristics of the coordinate values of each boundary node, and adding them to the specified boundary node list;

4) By traversing the element list of the above-mentioned finite element model, according to the relationship between the node coordinates of the elements and the characteristics of the node coordinates on the boundary, find the boundary element, and add it to the specified boundary element list;

5) Traverse the specified boundary node list, and take out any four nodes A, B, C and D among them, and judge whether these four nodes are four nodes on the first surface of the near field of the boundary infinite element;

6) If the four nodes A, B, C and D are the four nodes on the first surface of the near field of the boundary infinite element, then calculate the vector angle relationship according to the quantity product of the vectors to determine the relative position relationship of the four nodes;

7) Use the vector product between the vectors to determine the arrangement order of the four nodes in the counterclockwise direction as Q1, Q2, Q3, Q4;

8) The serial number of the infinite unit is determined by the number a of Part units specified in the finite model, the number of infinite units at the defined boundary is b, and the definition order c of infinite units in this area, then the current infinite unit number is Q=a+b+c;

9) Give the data line output of the infinite element definition of the specified boundary element:

Q,Q1,Q2,Q3,Q4,Q1+N,Q2+N,Q3+N,Q4+N

Among them: Q is the infinite element unit number, Q1, Q2, Q3, Q4 are four nodes in the near field, Q1+N, Q2+N, Q3+N, Q4+N are four nodes in the far field;

10) Two ways to output infinite unit definition data lines, the former mainly uses keyword line ① and data line ① for infinite unit definition, that is, the unit definition data line is directly inserted into the next line at the keyword definition position in Job-4.inp and save;

The latter mainly uses the keyword line ② and the data line ② for the infinite unit definition, writes the data line defined by the unit into the INPUT parameter filename.inp file in the infinite unit definition line, and ABAQUS will automatically read the filename when importing the model A row of data in the .inp file, generating infinite cells.

Further, traverse the specified boundary node list, and take out any four nodes among them, and judge whether the node is the four nodes on the first surface of the near field of the infinite element model. The specific steps are as follows:

Using the membership test function of Python, if the four nodes taken from the boundary node list are four nodes of the boundary element composition nodes, these four nodes are considered to be the four near-field nodes on the first surface of the boundary infinite element.

If the four nodes A, B, C and D are the four nodes on the first surface of the near field of the boundary infinite element, calculate the angle between the two vectors according to the vector quantity product to determine the relative position relationship of the four nodes, the specific steps include:

Taking point A as the first point of the quadrilateral, use the vector quantity product to calculate the sizes of ∠BAC, ∠BAD and ∠CAD respectively and sum them:

Let SUM=∠BAC+∠BAD+∠CAD:

1) If SUM=2∠BAC, then point A and point D, point B and point C are mutually diagonal nodes, and the counterclockwise order of nodes is A, B, D, C or A, C, D, B;

2) If SUM=2∠BAD, then point A and point C, point B and point D are mutually diagonal nodes, and the counterclockwise order of nodes is A, B, C, D or A, D, C, B;

3) If SUM=2∠CAD, then point A and point B, point C and point D are mutually diagonal nodes, and the counterclockwise order of nodes is A, D, B, C or A, C, B, D.

Using the vector product between vectors to determine the arrangement order of the four nodes in the counterclockwise direction, the specific steps include:

After determining the relative positional relationship of the four near-field nodes P1, P2, P3, and P4 in the first plane of the boundary infinite element, two vectors are formed by connecting any three adjacent nodes of the four nodes end to end, assuming that P1 and P3 , P2 and P4 are the corner points of each other, starting from P1, the adjacent nodes must be P2 and P4, then the counterclockwise order of the above four nodes is P1, P2, P3, P4 or P1, P4, P3, P2 , to calculate the vector and vector product of

like and the normal vector of point P1 on the current boundary surface When the included angle is an acute angle, that is:

Then the points P1, P2, and P3 are arranged counterclockwise, and the counterclockwise arrangement order of the four nodes is P1, P2, P3, P4;

like and the normal vector of point P1 on the current boundary surface When the included angle is obtuse, that is:

Then the points P1, P2, and P3 are arranged in a clockwise direction, and the counterclockwise arrangement order of the four nodes is P1, P4, P3, and P2.

Further, open the above INP file (Job-4.inp) by importing the ABAQUS model, and ABAQUS specifies that the Part 3D infinite unit boundary is automatically generated. The specific steps include:

Open ABAQUS/CAE, open the INP file (Job-4.inp) under the target folder through the model import method (Import→Model) under the File menu, and complete the modeling process of the boundary infinite element, which can be viewed under the specified Part Infinite element modeling effect.

Compared with the prior art, the beneficial effect of the present invention is: this method is mainly according to the unit node definition rule in ABAQUS three-dimensional infinite unit, utilizes the unit and node definition method of ABAQUS input file (. The programming completes the automatic output of the infinite element definition data line, completes the input file of the model definition according to the grammar rules of the INP file, and imports it into ABAQUS/CAE to generate the boundary infinite element. The embodiment of the invention is simple to operate, avoids the cumbersome process of manually modifying the INP file in the traditional method, has a high degree of automation, can generate infinite unit grids in a relatively short period of time, and greatly improves the modeling efficiency of ABAQUS.

Description of drawings

Fig. 1 is a flow chart of the technical solution of the present invention.

Figure 2 is the three-dimensional finite element model of ABAQUS.

Figure 3 is an infinite element far-field node generated by *NCOPY.

Figure 4 is an effect diagram of generating an infinite unit.

Figure 5 is the infinite element in the boundary area of the bottom surface of the model.

Figure 6 is the infinite element in the boundary area on the left side of the model.

Figure 7 is the infinite element in the boundary area on the right side of the model.

Figure 8 is the infinite element in the back boundary area of the model.

Figure 9 is the infinite element in the boundary area of the front end of the model.

detailed description

The present invention will be further described in detail below in conjunction with the accompanying drawings and specific embodiments.

As shown in Figure 1, the ABAQUS three-dimensional infinite element boundary fast modeling method based on INP file in the embodiment of the present invention comprises:

The three-dimensional model completed based on the three-dimensional unit grid division, and the rear center point of the three-dimensional model is located on the origin of the coordinate system, and the X axis, the Y axis and the Z axis of the coordinate system are its symmetry axes;

101. Establish the finite element model and create the specified Part boundary node set as the near-field node set of the infinite element, and export the ABAQUS input file (Job-1.inp);

Establish the ABAQUS/CAE three-dimensional finite element model as shown in Figure 2. According to the research problem, use the set tool under the Part module to establish the node set on the boundary surface of the specified Part as the near-field node corresponding to the boundary infinite element (the first surface of the infinite element The four nodes above) set, the node sets of different boundary areas are shown in Table 1; under the Job module, the analysis task Job-1 is established for the model of the above problem, and the ABAQUS input file is exported through Write Input on the Job Manager (Job-1.inp).

102. Modify the INP file and use the keyword (*NCOPY) to define the far-field nodes of the infinite element, and save it as a new INP file (Job-2.inp);

Modify the above INP file Job-1.inp, insert multi-line node definition keywords (*NCOPY) in the specified Part definition line according to different boundary areas, the command is as follows

*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

Use the keyword (*NCOPY) to copy the near-field nodes and offset the specified distance to generate the far-field node sets of infinite elements in different regions, as shown in Table 2. Save the above modified INP file as a new INP file (Job-2.inp) .

By copying the near-field nodes and offsetting a certain distance, define the far-field nodes of the infinite element boundary. The node number of the new node is based on the original node number by adding an integer value N to realize the near-field nodes and far-field nodes in the same infinite element extending in the direction of the infinite element. One-to-one correspondence, and the difference between the unit numbers is N. The selection of the N value should be combined with the selection of the total number of nodes in the model to ensure that the original finite element node numbers and the newly generated node numbers are not duplicated. The data line defines the coordinate offset value of the newly created far-field node based on the original near-field node.

Table 1 Infinite element near-field and far-field node sets in different boundary regions

103. Abaqus/CAE imports the modified INP file (Job-2.inp), checks the generated infinite element far-field nodes and exports the new INP file (Job-3.inp);

Import the modified INP file (Job-2.inp) through the graphical user interface GUI of Abaqus/CAE in the form of File→Import→Model, and generate the far-field nodes of the infinite element. Under the condition of the Part module, through View→PartDisplay Options →Click Show Node Labels under Mesh to display the unit node number, and you can view the generated infinite element far-field nodes in different regions, as shown in Figure 3, import the above model into the Job module, create a new Job-3 task, and pass the Write Input exports a new INP file (Job-3.inp).

104. INP file (Job-3.inp) inserts the keyword line (*ELEMENT) at the specified position to define the infinite unit, and save it as Job-4.inp;

Edit the INP file (Job-3.inp) according to the grammatical rules of the INP file of ABAQUS, define a new unit through the *ELEMENT keyword line and data line, and the insertion position of the keyword line and data line defined by the above unit must be at the infinite element boundary Before the definition end line of the Part where the *End Part keyword is located, after the far-field node set definition data line and the finite element element definition data line.

The INP file of ABAQUS mainly defines the infinite element through the *ELEMENT keyword, specifies the element type as CIN3D8, and establishes the infinite boundary element set on the corresponding boundary area; its data line is the specified element number and the node number composed of the element, for the three-dimensional infinite element ABAQUS The help document gives its definition rules, and this data line can also be read from other INP files that contain unit definition data.

The arrangement order of the node numbers defined by the above-mentioned data line unit meets the order of the nodes defined by the three-dimensional infinite unit (CIN3D8) in the ABAQUS help document.

In ABAQUS's INP file, *ELEMENT is used to define infinite units in two ways:

1) The data line defined by the infinite element is directly inserted into the next line where the keyword of the infinite element definition is located in 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) The data line defined by the infinite element is given by the external file filename.inp. The content of this file is only the data line defined by the current boundary area including the pre-completed input—including the infinite element 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

105.Python programming constructs the infinite element boundary cell definition data line and inputs it to the ABAQUS input file (Job-4.inp) or the specified INP file. The specific process is:

1) Use Python programming to read the node numbers and corresponding coordinates, unit numbers and component node numbers in the ABAQUS input file (Job-4.inp), and store them in the specified list;

2) Use Python programming to read the keyword line number defined by the infinite unit in the input file (Job-4.inp) of ABAQUS and store it in the specified variable, or read the INPUT parameter filename written by the infinite unit definition data line. inp;

3) Traversing the node list of the above-mentioned finite element model according to the characteristics of node coordinates, searching for nodes on different boundaries according to the characteristics of the coordinate values of each boundary node, and adding them to the specified boundary node list;

4) By traversing the element list of the above-mentioned finite element model, according to the relationship between the node coordinates of the elements and the characteristics of the node coordinates on the boundary, find the boundary element, and add it to the specified boundary element list;

5) Traverse the specified boundary node list, and take out any four nodes A, B, C and D among them, and judge whether these four nodes are four nodes on the first surface of the near field of the boundary infinite element;

6) If the four nodes A, B, C and D are the four nodes on the first surface of the near field of the boundary infinite element, then calculate the vector angle relationship according to the quantity product of the vectors to determine the relative position relationship of the four nodes;

7) Use the vector product between the vectors to determine the arrangement order of the four nodes in the counterclockwise direction as Q1, Q2, Q3, Q4;

8) The serial number of the infinite unit is determined by the number a of Part units specified in the finite model, the number of infinite units at the defined boundary is b, and the definition order c of infinite units in this area, then the current infinite unit number is Q=a+b+c;

9) Give the data line output of the infinite element definition of the specified boundary element:

Q,Q1,Q2,Q3,Q4,Q1+N,Q2+N,Q3+N,Q4+N

Among them: Q is the infinite element unit number, Q1, Q2, Q3, Q4 are four nodes in the near field, Q1+N, Q2+N, Q3+N, Q4+N are four nodes in the far field;

10) Two ways to output infinite unit definition data lines, the former mainly uses keyword line ① and data line ① for infinite unit definition, that is, the unit definition data line is directly inserted into the next line at the keyword definition position in Job-4.inp and save;

The latter mainly uses the keyword line ② and the data line ② for the infinite unit definition, writes the data line defined by the unit into the INPUT parameter filename.inp file in the infinite unit definition line, and ABAQUS will automatically read the filename when importing the model The rows of data in the .inp file generate infinite cells.

106. Open the above INP file (Job-4.inp) by importing the ABAQUS model, and the boundary of the three-dimensional infinite unit specified by ABAQUS is automatically generated.

Open ABAQUS/CAE, open the INP file (Job-4.inp) under the target folder through the model import method (Import→Model) under the File menu, and complete the modeling process of the boundary infinite element, which can be viewed under the specified Part The effect of infinite element modeling is shown in Figure 4. Figures 5-9 are generated infinite cell diagrams for different boundary regions.

Claims (10)

1. A fast modeling method of ABAQUS three-dimensional infinite element boundary based on INP file, it is characterized in that, according to the unit node definition rule in ABAQUS three-dimensional infinite element, utilize the unit and node definition method of ABAQUS input file .inp, realize by Python programming ABAQUS infinite element defines the automatic output of data lines, completes the input file of model definition according to the syntax rules of the INP file, and imports ABAQUS/CAE to generate boundary infinite elements; the specific steps include: Establish the finite element model and create the specified Part boundary node set as the near-field node set of the infinite element, and export the ABAQUS input file Job-1.inp; Modify the INP file and use the keyword *NCOPY to define the far-field nodes of the infinite element, and save it as a new INP file Job-2.inp; Abaqus/CAE imports the modified INP file Job-2.inp, checks the generated infinite element far-field nodes and exports the new INP file Job-3.inp; Insert the keyword line *ELEMENT to define the infinite element at the specified position in the INP file Job-3.inp, and save it as Job-4.inp; Python programming constructs the infinite element boundary cell definition data line and inputs it to the input file Job-4.inp of ABAQUS or the specified INP file; Open the INP file Job-4.inp by importing the ABAQUS model, and the boundary of the 3D infinite unit specified by ABAQUS is automatically generated. 2. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 1, is characterized in that, Establish the infinite element near-field node set in the finite element model and export the ABAQUS input file Job-1.inp including: Establish the ABAQUS/CAE three-dimensional finite element model, use the set tool under the Part module to establish the node set on the boundary surface of the specified Part as the near-field node set corresponding to the boundary infinite element, that is, the four nodes on the first surface of the infinite element nodes; Establish the analysis task Job-1 for the model of the research problem under the Job module, and export the ABAQUS input file Job-1.inp through Write Input on the Job Manager; Modify the INP file and use the keyword *NCOPY to generate the far-field nodes of the infinite element, and save it as a new INP file Job-2.inp including: Modify the INP file Job-1.inp, and insert the multi-line node definition keyword *NCOPY in the specified Part definition line according to different boundary areas; Use the keyword *NCOPY to form far-field nodes of infinite elements on the boundary of different regions; Save the modified INP file as a new INP file Job-2.inp; Abaqus/CAE imports the modified INP file Job-2.inp, checks the generated infinite element far-field nodes and exports the new INP file Job-3.inp including: Import the modified INP file Job-2.inp through the Abaqus/CAE graphical user interface GUI in the form of File→Import→Model, and the far-field nodes of the infinite element are generated, but they cannot be displayed temporarily; Under the condition of the Part module, click Show NodeLabels under View→Part Display Options→Mesh to display the unit node number, and view the generated infinite element far-field nodes in different regions; Put the import model in the Job module, create a new Job-3 task, and export the new INP file Job-3.inp through Write Input on the Job Manager; The INP file Job-3.inp inserts the keyword line *ELEMENT to define the infinite element at the specified position, and save it as Job-4.inp including: Edit the INP file Job-3.inp, insert the keyword line *ELEMENT in the specified line to define the infinite element; The INP file after inserting the *ELEMENT keyword row and the data row is saved as a new INP file Job-4.inp. 3. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 2, is characterized in that, utilizes keyword * NCOPY to generate the far-field node of different regional boundary infinite elements comprising: The keyword line and data line defined by the node must be edited according to the syntax rules of the INP file of ABAQUS; New nodes are defined via the *NCOPY keyword line and the data line. 4. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 3, is characterized in that, keyword row and data row must be edited according to the grammatical rule of the INP file of ABAQUS and comprise: 1) The far-field node defines the Keyword Line as: *NCOPY,CHANGE NUMBER=N,OLD SET=near_field_NodeSetName,NEW SET=far_field_NodeSetName,SHIFT 2) The far-field node defines the Data Line as: Shifting-x, Shifting-y, Shifting-z The keyword row and data row insertion position defined by the node must be located before the definition end row *End Part keyword of the Part where the infinite element boundary is located, and after the near-field node set defines the data row; New nodes defined by the *NCOPY keyword line and data line include: By copying the near-field node and offsetting a certain distance, define the far-field node of the infinite element boundary, and the node number of the new node is increased by the integer value N on the basis of the original node number; One-to-one correspondence between near-field nodes and far-field nodes along the infinite element direction of the same infinite element is realized, and the element numbers differ by N; The data line defines the coordinate offset value of the newly created far-field node based on the original near-field node. 5. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on the INP file according to claim 2 is characterized in that, editing the INP file Job-3.inp, inserting the keyword *ELEMENT line at the specified position to carry out the infinite element definition includes : Define infinite elements via the *ELEMENT keyword row and data row; The keyword line and data line defined by the infinite unit must be edited according to the syntax rules of the INP file of ABAQUS; The insertion position of the keyword line and data line defined by the node must be before the *End Part keyword of the definition end line of the Part where the infinite element boundary is located, and after the far-field node set definition data line and the finite element unit definition data line. 6. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 3, is characterized in that, defines boundary infinite element by *ELEMENT keyword line and data row and comprises: The definition of ABAQUS units and nodes is mainly through its pre-processor ABAQUS/CAE, creating geometric shapes and dividing unit grids to form unit nodes. The ABAQUS infinite units here are defined in the INP file by manually editing the INP file and inserting * The ELEMENT keyword assigns the unit number to the infinite unit, defines the unit by specifying the unit node number, and groups the boundary infinite elements at the same time; Considering that the unit number allocated on the assembly part is not unique, it needs to be distinguished in combination with the part Part, and the unit number allocated on the part is unique, so the definition of the boundary infinite element is only defined in the specified Part; Mainly define the infinite element through the *ELEMENT keyword, specify the element type as CIN3D8, and establish an infinite boundary element set on the corresponding boundary area; The data line defined by the infinite unit is the specified unit number and the node number composed of the unit; Abaqus infinite cell definition data line or read from other INP files containing cell definition data; The arrangement order of the node numbers defined by the data row unit meets the order of the nodes defined by the three-dimensional infinite unit CIN3D8 in the ABAQUS help document; The keyword line and data line defined by the infinite unit must be edited according to the grammar rules of the INP file of ABAQUS, including: 1) There are two ways of Keyword Line defined by Infinite Element Boundary Infinite Element, which are: ①*Element, type=CIN3D8, Elset=Infinite_Element_SetName ②*Element, type=CIN3D8, Elset=Infinite_Element_SetName, INPUT=filename.inp 2) The corresponding infinite unit defines the data line Data Line in two ways, corresponding to the keyword line: ①The data line defined by the infinite element is directly inserted into the next line where the keyword of the infinite element definition in the corresponding area is located, mainly including the infinite element number and the component node number, namely: Infinite_element_Num, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8 ②The data line defined by the infinite unit is given by filename.inp, and the content of this file only includes the data line defined by the infinite unit in the current boundary area that has been input in advance—including the infinite unit number and the component node number, namely: Infinite_element_Num, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8. 7. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 6, is characterized in that, the data row Infinite_element_Num of infinite element definition, NodeP1, NodeP2, NodeP3, NodeP4, NodeP5, NodeP6, NodeP7, NodeP8 include: The node numbers of the four nodes in the far field are N greater than the node numbers of the near-field nodes (nodes on the finite element boundary) corresponding to the edge of the element along the infinite direction, that is: <mfenced open = "{" close = ""> <mtable> <mtr> <mtd> <mrow> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>1</mn> <mo>+</mo> <mi>N</mi> <mo>=</mo> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>5</mn> </mrow> </mtd> </mtr> <mtr> <mtd> <mrow> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>2</mn> <mo>+</mo> <mi>N</mi> <mo>=</mo> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>6</mn> </mrow> </mtd> </mtr> <mtr> <mtd> <mrow> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>3</mn> <mo>+</mo> <mi>N</mi> <mo>=</mo> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>7</mn> </mrow> </mtd> </mtr> <mtr> <mtd> <mrow> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>4</mn> <mo>+</mo> <mi>N</mi> <mo>=</mo> <mi>N</mi> <mi>o</mi> <mi>d</mi> <mi>e</mi> <mi>P</mi> <mn>8</mn> </mrow> </mtd> </mtr> </mtable> </mfenced> According to the definition rules of the infinite element, the four nodes NodeP1, NodeP2, NodeP3 and NodeP4 in the near field of the first surface of the infinite element must meet the order of the four nodes in the near field in the counterclockwise direction when observing from the far field to the near field of the infinite element; The unit number specified 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 infinite unit definitions in the area. 8. the ABAQUS three-dimensional infinite element boundary fast modeling method based on INP file according to claim 7, is characterized in that, utilizes Python programming to construct infinite element boundary unit definition data line and input to the input file Job-4.inp of ABAQUS Or the specified INP file includes the following steps: 1) Use Python programming to read the node numbers and corresponding coordinates, unit numbers and component node numbers in the ABAQUS input file Job-4.inp, and store them in the specified list; 2) Use Python programming to read the keyword line number defined by the infinite unit in the ABAQUS input file Job-4.inp and store it in the specified variable, or read the INPUT parameter written by the infinite unit definition data line—ABAQUS read The INP file filename.inp; 3) Traverse the node list of the finite element model according to the node coordinate characteristics, search for nodes on different boundaries according to the characteristics of the coordinate value of each boundary node, and add to the specified boundary node list; 4) By traversing the element list of the finite element model, according to the relationship between the node coordinates of the elements and the characteristics of the node coordinates on the boundary, find the boundary element and add it to the specified boundary element list; 5) traverse the specified boundary node list, and take out any four nodes A, B, C, and D among them, and judge whether these four nodes are four nodes on the first surface of the near field of the boundary infinite element; 6) If the four nodes A, B, C and D are the four nodes on the first surface of the near field of the boundary infinite element, then calculate the vector angle relationship according to the quantity product of the vectors to determine the relative position relationship of the four nodes; 7) Utilize the vector product between the vectors to determine that the arrangement order of the counterclockwise direction of the four nodes is Q1, Q2, Q3, Q4; 8) The serial number of the infinite unit is determined by the number a of Part units specified in the finite model, the number of infinite units at the defined boundary is b, and the definition order c of infinite units in this area, then the current infinite unit number is Q=a+b+c; 9) Give the data line output of the infinite element definition of the specified boundary element: Q,Q1,Q2,Q3,Q4,Q1+N,Q2+N,Q3+N,Q4+N Among them: Q is the infinite element unit number, Q1, Q2, Q3, Q4 are four nodes in the near field, Q1+N, Q2+N, Q3+N, Q4+N are four nodes in the far field; 10) Two ways to output infinite unit definition data lines, the former mainly uses keyword line ① and data line ① for infinite unit definition, that is, the unit definition data line is directly inserted into the next line at the keyword definition position in Job-4.inp and save; The latter mainly uses the keyword line ② and the data line ② for the infinite unit definition, writes the data line defined by the unit into the INPUT parameter filename.inp file in the infinite unit definition line, and ABAQUS will automatically read the filename when importing the model A row of data in the .inp file, generating infinite cells. 9. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 8, is characterized in that, traverses specified boundary node list, and takes out wherein any four nodes, judges whether this node is infinite element model near The four nodes on the first face of the field include: Using the membership test function of Python, if the four nodes taken from the boundary node list are four nodes of the boundary element composition nodes, then these four nodes are the four near-field nodes on the first surface of the boundary infinite element; If the four nodes A, B, C, and D are the four nodes on the first surface of the near field of the boundary infinite element, the relative position relationship of the four nodes is determined by calculating the angle between the two vectors according to the vector quantity product: Taking point A as the first point of the quadrilateral, use the vector quantity product to calculate the sizes of ∠BAC, ∠BAD and ∠CAD respectively and sum them: <mfenced open = "{" close = ""> <mtable> <mtr> <mtd> <mrow> <mo>&amp;angle;</mo> <mi>B</mi> <mi>A</mi> <mi>C</mi> <mo>=</mo> <mfrac> <mrow> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>B</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>&amp;CenterDot;</mo> <mover> <mrow> <mi>A</mi> <mi>C</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> </mrow> <mrow> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>B</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>C</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> </mrow> </mfrac> </mrow> </mtd> </mtr> <mtr> <mtd> <mrow> <mo>&amp;angle;</mo> <mi>B</mi> <mi>A</mi> <mi>D</mi> <mo>=</mo> <mfrac> <mrow> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>B</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>&amp;CenterDot;</mo> <mover> <mrow> <mi>A</mi> <mi>D</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> </mrow> <mrow> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>B</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>D</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> </mrow> </mfrac> </mrow> </mtd> </mtr> <mtr> <mtd> <mrow> <mo>&amp;angle;</mo> <mi>B</mi> <mi>A</mi> <mi>C</mi> <mo>=</mo> <mfrac> <mrow> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>D</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>&amp;CenterDot;</mo> <mover> <mrow> <mi>A</mi> <mi>C</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> </mrow> <mrow> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>D</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> <mo>|</mo> <mover> <mrow> <mi>A</mi> <mi>C</mi> </mrow> <mo>&amp;RightArrow;</mo> </mover> <mo>|</mo> </mrow> </mfrac> </mrow> </mtd> </mtr> </mtable> </mfenced> Let SUM=∠BAC+∠BAD+∠CAD: 1) If SUM=2∠BAC, then point A and point D, point B and point C are mutually diagonal nodes, and the counterclockwise order of nodes is A, B, D, C or A, C, D, B; 2) If SUM=2∠BAD, then point A and point C, point B and point D are mutually diagonal nodes, and the counterclockwise order of nodes is A, B, C, D or A, D, C, B; 3) If SUM=2∠CAD, then point A and point B, point C and point D are mutually diagonal nodes, and the counterclockwise order of nodes is A, D, B, C or A, C, B, D; Using the vector product between vectors to determine the counterclockwise order of the four nodes includes: After determining the relative positional relationship of the four near-field nodes P1, P2, P3, and P4 in the first plane of the boundary infinite element, two vectors are formed by connecting any three adjacent nodes of the four nodes end to end, assuming that P1 and P3 , P2 and P4 are mutual corner points, starting from P1, the adjacent nodes must be P2 and P4, then the counterclockwise order of the four nodes is P1, P2, P3, P4 or P1, P4, P3, P2, Calculate vector and vector product of like and the normal vector of point P1 on the current boundary surface When the included angle is an acute angle, that is: <mrow> <mover> <mi>n</mi> <mo>&amp;RightArrow;</mo> </mover> <mo>&amp;CenterDot;</mo> <mover> <mi>p</mi> <mo>&amp;RightArrow;</mo> </mover> <mo>&gt;</mo> <mn>0</mn> </mrow> Then the points P1, P2, and P3 are arranged in a counterclockwise direction, and the counterclockwise arrangement order of the four nodes is P1, P2, P3, and P4; like and the normal vector of point P1 on the current boundary surface When the included angle is obtuse, that is: <mrow> <mover> <mi>n</mi> <mo>&amp;RightArrow;</mo> </mover> <mo>&amp;CenterDot;</mo> <mover> <mi>p</mi> <mo>&amp;RightArrow;</mo> </mover> <mo>&lt;</mo> <mn>0</mn> </mrow> Then the points P1, P2, and P3 are arranged in a clockwise direction, and the counterclockwise arrangement order of the four nodes is P1, P4, P3, and P2. 10. the ABAQUS three-dimensional infinite element boundary rapid modeling method based on INP file according to claim 7, it is characterized in that, open described INP file Job-4.inp by the mode of ABAQUS model import, ABAQUS specifies Part three-dimensional infinite element The automatic boundary generation includes: Open ABAQUS/CAE, through the model import method Import→Model under the File menu, open the INP file Job-4.inp under the target folder, complete the modeling process of the boundary infinite element, and view the infinite element modeling effect under the specified Part .