- Create elements.
From the main menu, select [Node/Element] tab > [General] group > [Create] > [Create Element]
Create Elements dialog box
Click to the right of Create Elements
Display the Element Table
Assign a number to the new starting node created together with new elements in the Model Window. This number is auto-set to the largest node number in use +1. To modify this item, click and select an option to specify a desired number.
Assign a new starting element number. This number is auto-set to the largest element number in use +1. To modify this item, click and select an option to specify a desired number.
Specify the element type and enter additional data.
Truss : Truss Element
The usage and precautions of truss elements(Truss/Comp.Only/Tens.Only)
Truss elements are primarily used for modeling components, such as space trusses, cables, and diagonal members, that primarily use forces along their axis or contact surfaces. These elements are commonly used in modeling structural elements that solely endure forces in the axial direction.
For example, truss elements can be used in modeling truss structures that can endure both compression and tension along their axis. Tension-only elements can be used in components such as cables or diagonal members where sagging can be ignored, or in elements like wind bracing where the compression forces are significantly smaller due to slenderness ratio.
Because these elements do not retain rotational degrees of freedom at nodes, Singular Errors can occur during the analysis at nodes where they are connected to the same type of elements or to elements without rotational d.o.f. MIDAS/Civil prevents such singular errors by restraining the rotational d.o.f. at the corresponding nodes.
If they are connected to beam elements that have rotational degrees of freedom, this restraining process is not necessary.
As shown in <Figure 1>, you should exercise caution not to induce unstable structures when only truss elements are connected. The structure shown in <Figure 1> (a) lacks rotational stiffness while being subjected to an external load in its plane, resulting in an unstable condition. <Figure 1> (b) and (c) illustrate unstable structures in the loading direction (X-Z plane), even though the structures are stable in the Y-Z plane direction.
You should use tension-only and compression-only elements with care. Element stiffness may be ignored in the analysis depending on the magnitudes of loads; e.g., when compression loads are applied to tension-only elements.
<Figure 1> Typical examples of unstable structures that are composed of truss
Tension only/Hook/Cable : Tension-only Elements
Tension only Truss
Allow. Comp : Allowable maximum compressive force
Tens. Limit : Allowable tensile force used in the process of iterative analysis
For tension-only elements, Allow Comp. is assigned 0 and Tens. Limit is checked off generally. If Tens. Limit is checked on and a specific value is entered, the element no longer resists forces exceeding the Tens. Limit, and the excess forces will be transferred to neighboring elements.
Hook : If a displacement takes place beyond the Hook Distance, the element starts resisting tension
Cable : enter the ratio of unstrained length of unstrained length to element length (Lu/L) and the Pretension load additionally. "Cable Element" is auto-converted into equivalent Truss Element in the case of a linear analysis and Elastic Catenary Element in the case of a geometric nonlinear analysis.
Lu : Enter the unstrained length of Cable (Lu), which will indirectly adjust element stiffness and tension force from element length. (Lu: Unstrained length of Cable, L: Element length)
Pretension : Enter the Pretension load to be introduced to Cable.
Horizontal : Enter the Horizontal pretension load, which will be automatically converted into the pretension load to be introduced to Cable.
Entered pretension is applied only when nonlinear analysis is performed. Unless geometric nonlinear analysis is performed, the entered pretension will be ignored. For linear analysis, pretension should be entered using Load>Prestress Loads> Pretension Loads.
Compression only/Gap : Compression-only Elements
Compression only Truss
Allow. Tens : Allowable maximum tensile force
Comp. Limit : Allowable compressive force used in the process of iterative analysis
For compression-only elements, Allow Tens. is assigned 0 and Comp. Limit is checked off generally. If Comp. Limit is checked on and a specific value is entered, the element no longer resists forces exceeding the Comp. Limit, and the excess forces will be transferred to neighboring elements.
Gap : If a displacement takes place beyond the Gap Distance, the element starts resisting compression.
General beam/Tapered Beam : Beam Element/Non-prismatic Beam Element
The usage and precautions of Beam Element/Non-prismatic Beam Element
This element is typically used for modeling prismatic and non-prismatic tapered structural members that are relatively long compared to section dimensions. The element can be also used as load-transfer elements connecting other elements having differing numbers of d.o.f.
In-span concentrated loads, distributed loads, temperature gradient loads and prestress loads can be applied to beam elements.
A beam element has 6 d.o.f. per node reflecting axial, shear, bending and torsional stiffness. When shear areas are omitted, the corresponding shear deformations of the beam element are ignored.
The beam element is formulated on the basis of the Timoshenko beam theory (a plane section initially normal to the neutral axis of the beam remains plane but not necessarily normal to the neutral axis in the deformed state) reflecting shear deformations. If the ratio of the section depth to length is greater than 1/5, a fine mesh modeling is desirable because the effect of shear deformations becomes significant.
The torsional resistance of a beam element differs from the sectional polar moment of inertia (they are the same for circular and cylindrical sections). You are cautioned when the effect of torsional deformation is large, as the torsional resistance is generally determined by experimental methods.
Beam and truss elements are idealized line elements, thus their cross-sections are assumed to be dimensionless. The cross-sectional properties of an element are concentrated at the neutral axis that connects the end nodes. As a result, the effects of panel zones between members (regions where columns and beams merge) and the effects of non-alignment of neutral axes are not considered. In order for those nodal effects to be considered, the beam end offset option or geometric constraints must be used.
The tapered section may be used when the section of a member is non-prismatic. It may be desirable to use a number of beam elements to model a curved beam.
When members are connected by pins or slotted holes (<Figure 2> (a) and (b)), the Beam End Release option is used.
Note that a singularity error can result in a case where a particular degree of freedom is released for all the elements joining at a node, resulting in zero stiffness associated with that degree of freedom. If it is inevitable, a spring element (or an elastic boundary element) having a minor stiffness must be added to the corresponding d.o.f.
(a) Pin connection
(b) Slotted hole connection
When several beam elements are pin connected at a node, the degree of freedom for at least one element must be maintained while the ends of all other elements are released in order to avoid singularity.
(d) When elements having different d.o.f. are connected
<Figure 2> Examples of end-release application
The rigid beam element can be effectively used when elements having different degrees of freedom are connected. The rigid effect is achieved by assigning a large stiffness value relative to the contiguous beam elements. In general, a magnitude of 10^5 ~ 10^8 times the stiffness of the neighboring elements provides an adequate result, avoiding numerical ill conditions.
<Figure 2> (d) illustrates the case where a beam member is joined to a wall. The wall element may be a plane stress or plate element. The nodal in-plane moment corresponding to the beam element's rotational degree of freedom will not be transmitted to the planar element (plane stress or plate element) because the planar element has no rotational stiffness about the normal direction to the plane. The interface will behave as if the beam was pin connected. In such a case, a rigid beam element is often introduced in order to maintain compatible connectivity. All degrees of freedom of the rigid beam at the beam element are fully maintained while the rotational and axial displacement degrees of freedom are released at the opposite end.
Plate : Plate Element
Thick : Thick plate element
Thin : Thin plate element
Thick and Thin plates are distinguished by whether or not shear deformation is considered. Refer to "Important Aspects of Element Selection" of Analysis Manual.
With Driling DOF : To consider the degree of freedom about the perpendicular direction to the plate
The usage and precautions of Plate Element
This element can be used to model the structures in which both in-plane and out-of-plane bending deformations are permitted to take place, such as pressure vessels, retaining walls, bridge decks, building floors and mat foundations.
Pressure loads can be applied to the surfaces of the elements in either the GCS or ECS.
A plate element can be either quadrilateral or triangular in shape where its stiffness is formulated in two directions, in-plane direction axial and shear stiffness and out-of-plane bending and shear stiffness.
The out-of-plane stiffness used in MIDAS/Civil includes two types of elements, DKT/DKQ (Discrete Kirchhoff elements) and DKMT/DKMQ (Discrete Kirchhoff-Mindlin elements). DKT/DKQ were developed on the basis of the Kirchhoff Thin Plate theory. Whereas, DKMT/DKMQ were developed on the basis of the Mindlin-Reissner Thick Plate theory, which results in superb performances on thick plates as well as thin plates by incorporating appropriate shear strain fields to resolve the shear-locking problem. The in-plane stiffness of the triangular element is formulated in accordance with the Linear Strain Triangle (LST) theory, whereas the Isoparametric Plane Stress Formulation with Incompatible Modes is used for the quadrilateral element.
The user may separately enter different thicknesses for an element for calculating the in-plane stiffness and the out-of-plane stiffness. In general, the self-weight and mass of an element are calculated from the thickness specified for the in-plane stiffness. However, if only the thickness for the out-of-plane stiffness is specified, they are calculated on the basis of the thickness specified for the out-of-plane stiffness.
Similar to the plane stress element, the quadrilateral element type is recommended for modeling structures with plate elements. When modeling a curved plate, the angles between two adjacent elements should remain at less than 10° Moreover, the angles should not exceed 2~3° in the regions where precise results are required.
It is thus recommended that elements close to squares be used in the regions where stress intensities are expected to vary substantially and where detailed results are required.
<Figure 3> Example of plate elements used for a circular or cylindrical modeling
Plane Stress : Plane Stress Element
With Driling DOF : To consider the degree of freedom about the perpendicular direction to the plate
The usage and precautions of Plane Stress Element
This element can be used for modeling membrane structures that are subjected to tension or compression forces in the plane direction only. Pressure loads can be applied normal to the perimeter edges of the plane stress element.
The plane stress element may retain a quadrilateral or triangular shape. The element has in-plane tension, compression and shear stiffness only.
Quadrilateral (4-node) elements, by nature, generally lead to accurate results for the computation of both displacements and stresses. On the contrary, triangular elements produce poor results in stresses, although they produce relatively accurate displacements. Accordingly, you are encouraged to avoid triangular elements at the regions where detailed analysis results are required, and they are recommended for the transition of elements only <Figure 4>.
Singularity errors occur during the analysis process, where a plane stress element is joined to elements with no rotational degrees of freedom since the plane stress element does not have rotational stiffness. In MIDAS/Civil, restraining the rotational degrees of freedom at the corresponding nodes prevents the singularity errors.
When a plane stress element is connected to elements having rotational stiffness such as beam and plate elements, the connectivity between elements needs to be preserved using the rigid link (master node and slave node) option or the rigid beam element option.
Appropriate aspect ratios for elements may depend on the type of elements, the geometric configuration of elements and the shape of the structure. However, aspect ratios close to unity (1:1) and 4 corner angles close to 90?are recommended. If the use of regular element sizes cannot be achieved throughout the structure, the elements should be square shaped at least at the regions where stress intensities are expected to vary substantially and where detailed results are required.
Relatively small elements result in better convergence.
<Figure 4> Crack modeling using quadrilateral/triangular elements
Plane Strain : 2-D Plane Strain Element
The usage and precautions of Plane Strain Element
This element can be used to model a long structure, having a uniform cross section along its entire length, such as dams and tunnels. The element cannot be used in conjunction with any other types of elements.
Pressure loads can be applied normal to the perimeter edges of the plane strain element.
Because this element is formulated on the basis of its plane strain properties, it is applicable to linear static analyses only. Given that no strain is assumed to exist in the thickness direction, the stress component in the thickness direction can be obtained through the Poisson's effect.
The plane strain element may retain a quadrilateral or triangular shape. The element has in-plane tension, compression and shear stiffness, and it has tension and compression stiffness in the thickness direction.
Similar to the plane stress element, quadrilateral elements are recommended over the triangular elements, and aspect ratios close to unity are recommended for modeling plane strain elements.(Refer to Create Element>Plane Stress Element.)
Axisymmetric : 2-D Axisymmetric Element
The usage and precautions of Axisymmetric Element
This element can be used for modeling a structure with axis symmetry relative to the geometry, material properties and loading conditions, such as pipes, vessels, tanks and bins. The element cannot be used in conjunction with any other types of elements.
Pressure loads can be applied normal to the circumferential edges of the axisymmetric element.
Because this element is formulated on the basis of its axisymmetric properties, it is applicable to linear static analyses only. It is assumed that circumferential displacements, shear strains and shear stresses do not exist.
Similar to the plane stress element, quadrilateral elements are recommended over the triangular elements, and aspect ratios close to unity are recommended for modeling axisymmetric elements.(Refer to Create Element>Plane Stress Element.)
Solid : 3-D Solid Element
The usage and precautions of 3-D Solid Element
This element is used for modeling three-dimensional structures, and its types include tetrahedron, wedge and hexahedron.
Pressure loads can be applied normal to the surfaces of the elements or in the X, Y, and Z-axes of the GCS.
The use of hexahedral (8-node) elements produces accurate results in both displacements and stresses. On the other hand, using the wedge (6-node) and tetrahedron (4-node) elements may produce relatively reliable results for displacements, but poor results are derived from stress calculations. It is thus recommended that the use of the 6-node and 4-node elements be avoided if precise analysis results are required. The wedge and tetrahedron elements, however, are useful to join hexahedral elements where element sizes change.
Solid elements do not have stiffness to rotational d.o.f. at adjoining nodes. Joining elements with no rotational stiffness will result in singular errors at their nodes. In such a case, MIDAS/Civil automatically restrains the rotational d.o.f. to prevent singular errors at the corresponding nodes.
When solid elements are connected to other elements retaining rotational stiffness, such as beam and plate elements, introducing rigid links (master node and slave node feature in MIDAS/Civil) or rigid beam elements can preserve the compatibility between two elements.
An appropriate aspect ratio of an element may depend on several factors such as the element type, geometric configuration, structural shape, etc. In general, it is recommended that the aspect ratio be maintained close to 1.0. In the case of a hexahedral element, the corner angles should remain at close to 90? It is particularly important to satisfy the configuration conditions where accurate analysis results are required or significant stress changes are anticipated. It is also noted that smaller elements converge much faster.
Select a material property number, or select a material property name provided that the material property data have been already defined.
No. : Type in a number on the keyboard or use the mouse to enter the number.
Name : Select a material property name.
Click to add, inquire, modify or delete material property data. Material properties can be entered either before or after creating elements.
Select a section (thickness) number, or select a section (thickness) name provided that the section (thickness) data have been already defined.
No. : Type in a number on the keyboard or use the mouse to enter the number.
Name : Select a section (thickness) name.
Click to add, inquire, modify or delete section (thickness) data. Section data can be entered either before or after creating elements.
When elements are of a line type (Truss, Beam, etc.), Beta Angle, the coordinates of Reference Point, or Reference Vector are specified to define the orientation of sections.
When using the Beta Angle, the direction from the N1 node to the N2 node becomes the x-axis of the element coordinate system.
If the coordinates of the Reference Point are entered, midas Civil internally computes the angle of the point and enters the angle as a Beta Angle automatically.
If the coordinates of the Reference Vector are entered, z-axis of an element is placed on the plane containing the Vector.
midas Civil uses the Beta Angle (β) conventions to identify the orientation of each cross-section. The Beta Angle relates the ECS to the GCS. The ECS x-axis starts from node N1 and passes through node N2 for all line elements. The ECS z-axis is defined to be parallel with the direction of "I" dimension of cross-sections. That is, the y-axis is in the strong axis direction. The use of the right-hand rule prevails in the process.
If the ECS x-axis for a line element is parallel with the GCS Z-axis, the Beta angle is defined as the angle formed from the GCS X-axis to the ECS z-axis. The ECS x-axis becomes the axis of rotation for determining the angle using the right-hand rule. If the ECS x-axis is not parallel with the GCS Z-axis, the Beta angle is defined as the right angle to the ECS x-z plane from the GCS Z-axis (See below).
|(a) Case of vertical members
(ECS x-axis is parallel with the global Z-axis)
|(b) Case of horizontal or diagonal members
(ECS x-axis is not parallel with the global Z-axis.)
Beta Angle Conventions
Enter the node numbers defining the element in accordance with the (N1, N2,?) sequence shown in the figure that appears upon selecting Element Type.
Use the following two methods to enter the element's nodal connectivity.
1. Type in the node numbers in the Nodal Connectivity field.
2. Click the Nodal Connectivity field, which will turn the background color to pale green. Then, assign consecutively the desired node points in the Model Window to enter elements. If there is no node at the assigned point, a new node is created. It is quite convenient to create elements when Point Grid (or Line Grid) , Grid Snap, Node Snap and Elements Snap. are activated. If Ortho option is selected the mouse cursor snaps to the entities oply in the directions parallel to the currently active coordinate axes (UCS or GCS) from the first point selected.
3. The nodal locations defining the new elements are entered by directional axes, relative distances or element lengths/angles.
x, y, z : The coordinates of the connecting point of an element are entered in the data entry field, then press the enter key on the keyboard or click En.
dx, dy, dz : Enter a distance relative to the reference point and press the enter key on the keyboard or click En, If characters are included in the string of numerical values, midas Civil recognizes them as a relative distance, irrespective of which one of the three methods of data entry is selected
Example : 'dx, dy, dz'의 '10, 20, 10' => '@10, 20, 10'
l, theta : l represents the length of an element. Theta represents the angle by which the element direction is rotated with respect to x-axis of the current coordinate system. Once the data are entered, press the enter key on the keyboard or click En.
Example : '10, 15' of 'l, theta' are expressed as '@10<15'
The origin of the current coordinate system is assigned as the reference point initially. Subsequently, the last point used becomes the reference point. To confirm the location of the reference point, enter '@0' in the data field and press the Enter key on the keyboard.
If Intersect Node is selected and existing nodes are on the element, the element is divided at the existing nodal positions irrespective of the element type.
If Intersect Element is selected and the line element created intersects with an existing line elements, nodes are automatically created and the line elements are divided at the intersections.
If Create Intersecting Nodes is selected and even if there are no interior nodes in the created plate and solid elements, nodes are created at the intersections of the lines extended by the exterior nodes and plate or solid elements are subsequently created.
Example of Create Intersecting Nodes application
Self-weight is applied like uniformly distributed load (external force) using element length, cross section area, and material weight density.
If we assume that uniformly distributed load is applied to the tens.-only truss element, above the half position will be in tension and the below the half position will be in compression. Due to the limitation of application in self-weight, tens.-only or comp.-only properties cannot be considered with self-weight.
As an alternative, we can apply the self-weight using static nodal load with changing weight density of material as zero. If the conversion of self-weight into nodal load is complex, we can also assign tension-only inelastic hinge (slip bilinear tension) in nonlinear static time history analysis.