2.7. Assign menu
Automatic loading: Allows to assign to all the elements in the model some automatic-generated loads, such as self-weight and wind loads.
The command Assign self-weight loads produces the distributed load only for the elements having a material and a section assigned to.
The command Assign in the Wind loads box produces the assignation of wind load to all the Line elements in the model, in the chosen direction. The loading is calculated from a defined user function, and applied to the lateral surface of each element, obtained from the largest edge of the transversal section.
Point load: Applies a concentrated loads to selected nodes. To insert a concentrate load:
- Select one or more nodes;
- Insert the loads value in the Load value box;
- Select the direction clicking in a radio-button on the Direction box;
- Select the load case on the Load case drop-down list;
- Click on the Apply button to set the load.
To use a value from a defined function, pick the desired function from the Pick function menu and then specify the value from which read the function the in the At X menu. Optionally, a multiplier for the resulting value can be specified.
Finally, the option Temperature allows to assign a nodal temperature to be used in Heat-transfer load cases.
Distributed load: To insert a distributed load on a line element:
- Insert the value of the load in Uniform load value box specifying the correct sign in global coordinate system;
- Select the Direction of the load;
- Select the proper Load case;
- Select the element in the model and click on the Apply button.
To remove a distributed in the selected load case, select the element in the model and click on the Remove button.
By the Non-uniform loading box it is possible to insert linear distributed load by points, specifying the proper distance for the input values.
WARNING: The units need to be consistent with the initial choices [Force/Length].
WARNING: Since version 1.3, non-uniform loading is supported even in the default solver. An indefinite number of multi-linear distributed loads can be applied on the same beam.
WARNING: Rigid offsets applied on beams having non-uniform loads must be placed before and/or after the beginning or the end of the loads, otherwise they will not be considered.
WARNING: Line3 elements, for compatibility reasons, do not support non-uniform loading. Line elements can be used without losing accuracy.
Temperature: Applies a thermal load, which causes a structural deformation, to the selected beams and planar elements. Beam element support the uniform gradient and the linear temperature gradient, in both y and z directions of the transversal cross section. Planar elements support only uniform gradient. Finally, solid elements do not support thermal loading.
Edge load: Applies an uniform load on an edge of an element. It can be used to assign forces per unit of length (Force option) or temperatures (Temperature option). This last option is intended to be used of heat transfer analysis only. After you selected the planar element, from the Select side box it is possible to highlight the chosen edges.
Non-uniform loading box allows to set a final value for load. The button Apply on path by selected nodes allows to apply edge loads following selected nodes.
Floor load: Applies a floor load on a triangular surface defined by Line elements or quadrangular by selecting 3 or 4 nodes. Choose the floor type within:
- Centroid-trilateral plane: to load a triangular plane distributing the load all over its sides;
- Centroid-quadrilateral plane: to load a quadrilateral plane distributing the load all over its sides;
- One-way quadrilateral plane: to load a quadrilateral plane on 2 or more sides taking into account the load direction (i.e. floor frames);
- Two-way quadrilateral plane: to load quadrilateral plane with 2-way distribution (tributary area method).
In the Set floor load mask target load cases and relatives values can be specified.
In the Load direction box it is possibile to specify a direction for applied loads. The default setting Normal to plane applies the loading normal to the plane by considering its clockwise or counterclockwise orientation. This setting will be ignored if another direction is specified.
To draw the plane once selected the desired plane load, select Draw plane.
WARNING: input loads in this section must have F/L2 dimension.
WARNING: edge plane elements can only be of Line type.
WARNING: the plane drawing direction defines the load sign (positive or negative) in the global coordinate system - draw planes counter clockwise to keep the value defined in the Set load table.
Pressure load: Applies a pressure load on planar elements.
The Non-uniform loading box allows to apply a bilinear load on a face of planar element.
Volume load: It applies a load per unit of volume on solid elements.
Point displacement: Applies displacements to selected nodes.
Initial temperature: Set the initial temperature in the model.
WARNING: This command affects only thermal analyses. It does not affect the loads induced by thermic distortion.
Pretension load: Applies pretension loads to linear (truss and beams) elements. A positive value signifies a tensioned element (i.e. tendons, cables). Only positive values are permitted (i.e. element in tension).
WARNING: The load is displayed as a uniform thermal distortion on the element. The value of distortion will have the opposite sign of the assigned pretension.
Point Mass: Applies masses to selected nodes.
WARNING: The units need to be consistent with the initial choices.
WARNING: You may want to add the nodal mass in all the three translational directions.
Masses from loads: Allows to transform, automatically or once at a time, the loads contained in a load case into masses. Checks in 'Set masses in' activate or deactivate the mass in the corresponding direction.
The "Assign nodal masses from loadcase" box is used for assigning masses in the directions specified above without changing them as loads change.
Material: Assigns material to the selected elements.
Section: Assigns section to the selected elements.
Local axes rotation: In the Beams box, the command rotates the selected beam sections by the counter-clockwise angle specified.
In the Planar Elements box, it rotates the planar local axes by changing the element connectivity.
The Reverse connectivity command is used to reverse the Z axes of plane elements.
NOTICE: With non-regular meshes (e.g., triangular), all local axes should be rectified in order to read the results in terms of stresses and strains consistently
Restraints: Assigns restraint to the degrees of freedom selected by checking the appropriate check box.
In viewport, the following drawing conventions applies:
x, y and z checked (simple support)
all checked (fixed end)
x, y, z and ry, rz blocked (fixed in XZ plane, simply supported in YZ plane)
y and z fixed, slider in plane xz
x, y, z and rx blocked
only ry blocked
rx and ry blocked
all other restraint types.
Constraints: Assign a constraint (i.e. rigid diaphragm or master-slave link) to selected nodes. By the Rigid diaphragm preset, a rigid floor can be applied to the selected nodes.
WARNING: The master node must be bounded properly to avoid singularities in the model. This procedure always proposes the proper boundary conditions automatically.
End releases: Assigns end releases to beam elements. By specifying a value between 0 (fully released) and 1 (fully fixed) in the textbox next to the check, a partial end release to be used in a linear elastic analysis can be obtained. The reduction factor r is applied to reduce the stiffness of the beam by the ratio r/(1-r).
The option “Input stiffnesses” allows to directly set stiffness values instead of force ratios.
Rigid offset: Assigns one or more rigid offsets to beam elements.
WARNING: Loads on a beam with rigid offsets are not modified not changed or adapted to the rigid segments. As a result, distributed loads on beams can decrease in their overall intensity due to the lesser length of application.
Element properties: Assigns custom properties to beam elements. For the property names and reserved values see chapter 4.
In addition, from this mask it’s possible to assign a beam section offset at element level, from the box Beam section offset.
Hinges: Assigns plastic hinges to beam elements. After the name of the hinge has been inserted, press Add. At this point, each DoF of the hinge can be set by inserting the properties listed below. Press Modify to save the hinge properties.
The Hinges options box allows to specify under which loading conditions all hinges have to be recalculated. This is particularly useful for hinges with NVM interaction.
Data requested for a Bilinear Symmetric plastic hinge are:
- Fy: strength at elastic limit;
- cKpl: coefficient to set the slope of the plastic branch Kpl=cKpl * Kel;
- m: hinge ductility;
- Fres/Fy: residual strength in percentage of Fy.
Data requested for a Bilinear Unsymmetrical plastic hinge are:
- Fy+: strength at elastic limit;
- cKpl+: coefficient to set the slope of the plastic branch Kpl=cKpl * Kel;
- m+: hinge ductility;
- Fres/Fy+: residual strength in percentage of Fy+
- All the above quantities followed by a “-” sign: to define the negative part of the hinge law.
The hinges inserted with Custom properties are defined by setting all the above data.
By selecting NVM from the DoF dropdown menu it is possible to assign an axial/shear/flexure interacting hinge. The calculation of all its properties is made automatically on the assignation on the base of checking type selected from the dropdown menu Hinge type. NVM hinges always have an unsymmetrical bilinear law.
Hinge status can be seen together with beam diagrams results, with the following convention.
Member: Assigns one or more elements to a member. This affects the verification of a beam element.
Rebars: Assigns reinforced bars to beam elements. By selecting the desired section from the Beam sections box, the potential rebar defined in Assign/Sections/Strength is shown and it can be applied to the beams having that section.
The table in the box named Assigned rebar shows the longitudinal and shear reinforcements assigned to each beam, or to a portion of a beam by specifying the Start at and Ends at values.
The Rebar position box allows to define and change longitudinal and shear reinforcements. Stirrups are defined in the Shear reinforcement sub-box. The Fast rebar positioning box allows to easily insert simple rebar schemes for the most common sections.
Span drawingshows the longitudinal section of the beam, highlighting the selected part.
WARNING: units of measure used in this mask are the same defined for the model, except for the diameters of the available bars in the dropdown menus, with are shown in mm.
Spring properties: Add, modify or assign one set of properties (elastic stiffnesses) for linear springs.
It is also possible to specify and assign subsoil distributed springs on beam elements (as elastic foundations) by using the box Elastic soil properties in Z direction by using the button Add soil spring after having set the Winkler’s modulus and the Beam width.
The Assign as nodal spring to selected nodes button allows to assign to a node the selected spring, connected to another fully fixed node that is automatically restrained.
The Assign springs to overlapped nodes command allows to easily assign zero-length springs to the selected overlapped nodes.
It is possible to assign non-linear properties for a translational (x, y, z) or rotational (rx, ry, rz) DoFs, either in global or local coordinates as specified in the upper right corner of the property box. By clicking on the NL checkbox, the non-linear properties dropdown will list all the hysteretic laws available. Select one item from the dropdown to set properties.
WARNING: in order to define the non-linear properties, it is necessary to add a spring property first. Once the non-linear properties have been defined, click on Modify property to store them.
The non-linear models available in NextFEM Designer are:
- Gap: gap spring is particularly useful for representing contact (i.e. gap with null opening). Such model works only in compression with the stiffness defined by the user.
Data requested for Gap are:
§ closure: maximum closure of the gap;
§ Kclosure: slope of the compression branch.
|
|
|
|
|
|
- Hook: this law reacts only in tension. Data requested for Hook are:
§ opening: displacement at which tension stiffness is not null;
§ Kopening: slope of the tension branch.
|
|
|
- Bilinear Plastic: the elastic behaviour is maintained until the yielding force Fy is reached, then the plastic field begins. Once the ultimate displacement Uu is achieved, the spring breaks, maintaining a residual force Fres. This law has a symmetrical behaviour.
|
|
|
Data requested for a Bilinear Plastic behaviour are:
§ Kel: elastic stiffness assigned to the spring;
§ Fy: strength at elastic limit;
§ cKpl: coefficient to set the slope of the plastic branch Kpl=cKpl * Kel;
§ Uu: ultimate displacement;
§ Fres: residual strength after collapse.
- Bilinear Unsymmetrical: this behaviour is suitable for modelling non-symmetric behaviour in structural elements. This law has an unsymmetrical behaviour.
|
|
|
Data requested for a Bilinear Unsymmetrical type behaviour are:
§ Kel+: elastic stiffness assigned to the spring;
§ Fy+: strength at elastic limit;
§ cKpl+: slope of the positive plastic branch;
§ Uu+: ultimate displacement allowed;
§ Fres+: residual force for
§ All the above quantities followed by “-“ are the same properties for the compression side.
- Trilinear Plastic: after reaching the plastic field, the skeleton curve is characterized by an hardening branch bringing to Fmax, followed by a hardening/softening one that leads to failure at Uu. This law may have or not a symmetrical behaviour.
|
|
|
Data requested for a Trilinear Plastic behaviour are:
§ Kel+: elastic stiffness assigned to the spring;
§ Fy+: strength at elastic limit;
§ Kp1+: slope of the first plastic branch;
§ Fmax: maximum strength reachable;
§ Kp2+: slope of the second plastic branch;
§ Uu+: ultimate displacement in positive direction;
§ All the above quantities (except Fmax) followed by “-“ are the ones for the compression side;
§ Fmin: maximum strength reachable in compression.
- Pivot rule: such model follows the rules defined in Dowell RK, Frieder S, Wilson LE. Pivot hysteresis model for reinforced concrete members. Struct J 1998;95(5):607–17. The law can be set as not symmetrical. The definitions of the pivot points can be made by setting the a and b parameters.
Referring to the Trilinear Plastic rule, the additional parameters are:
§ alpha1: sets the pivot point for unloading from a tensile force to zero;
§ beta1: sets the pivot point for reverse loading from zero to a negative force. Must be set between 0 and 1;
§ alpha2: sets the pivot point for unloading from a compressive force to zero;
§ beta2: sets the pivot point for reverse loading from zero to a positive force. Must be set between 0 and 1.
|
|
|
- Tomazevic-Lutman model: represents a trilinear behaviour as defined in Tomazevic M, Lutman M. Seismic behavior of masonry walls – modeling of hysteretic rules. J Struct Eng 1996:1048–54. It is influenced by parameters alpha and beta, which determine the stiffness and the strength degradations, respectively. This model is suitable for shear DoFs in masonry walls. This law has a symmetrical behaviour.
|
|
|
Data requested for Tomazevic-Lutman model are:
§ Kel: elastic stiffness assigned to the spring;
§ Fy: strength at elastic (cracking) limit;
§ Kpl1: slope of the first plastic branch;
§ Fmax: maximum strength reachable;
§ Kpl2: slope of the second hardening/softening plastic branch;
§ cF: coefficient to set unloading force ratio from the backbone;
§ alpha: coefficient for linear stiffness degradation at unloading (Kult=alpha*Kel);
§ beta: coefficient for strength degradation on the base of energy dissipated in a cycle (default 0.06);
§ Uu: ultimate displacement.
- Ring-shape: this model represent a poor dissipative cyclic behaviour and can be used, for example, for flexural DoFs in slender masonry panels. The backbone can be bilinear if Kpl2 is set to zero.
This law has a symmetrical behaviour.
|
|
|
Data requested for the Ring-shape model are:
§ Kel: elastic stiffness assigned to the spring;
§ Fy: strength at elastic (cracking) limit;
§ Kpl1: slope of the first plastic branch;
§ Fmax: maximum strength reachable;
§ cC: coefficient to set the slope of the unloading path;
§ cF: coefficient to set unloading force ratio from the backbone;
§ alpha: coefficient for linear stiffness degradation at unloading (Kult=alpha*Kel);
§ cD: way point for the unloading path - distance from elastic limit in backbone curve;
§ Uu: ultimate displacement;
§ Kpl2: slope of the seconnd plastic branch, can be set to 0 to remove it.
- Slip type: trilinear behaviour exploitable for shear connection in timber structures (nails, screws, angle brackets, ect.). Such law is based on the work Rinaldin G., Fragiacomo M. A Component Model for Cyclic Behaviour of Wooden Structures. Materials and joints in Timber structures: recent developments of technology, RILEM Bookseries, Vol. 9, pp. 519-530, 2014, DOI: 10.1007/978-94-007-7811-5_48, ISBN: 978-94-007-7811-5.
This law has a symmetrical behaviour.
|
|
|
Data requested for the Slip-type model are:
§ Kel: elastic stiffness assigned to the spring;
§ Fy: strength at elastic limit;
§ Kpl1: slope of the positive plastic branch, must be ≠0;
§ Fmax: maximum strength reachable;
§ Kpl2: slope of the negative plastic branch, must be ≠0;
§ cKunload: it sets the unloading stiffness of the first branch of unloading (green) and of reloading (blue) path by multiplying the elastic stiffness by this factor;
§ cFreload: it sets the lower limit of last branch of reloading (blue) and unloading (green) path, in percentage of the force value in the backbone. Such parameter must be set between 0 and 1;
§ cFunload: it sets the lower limit of first branch of unloading (green) and reloading (blue) path, in percentage of the force value in the backbone. Such parameter must be set between 0 and 1;
§ Uu: ultimate displacement;
§ alpha: exponential strength degradation parameter based on dissipated energy;
§ beta: exponential strength degradation parameter based on maximum displacement reached;
§ gamma: linear strength degradation parameter;
§ cKreload: sets the unloading stiffness of last branch of the reloading (blue) and unloading (green) path by multiplying the elastic stiffness by this factor.
- Unsymmetrical Slip-type: this behaviour is suitable for modelling hold-down connections in timber structures. Such law is based on the work Rinaldin G., Fragiacomo M. A Component Model for Cyclic Behaviour of Wooden Structures. Materials and joints in Timber structures: recent developments of technology, RILEM Bookseries, Vol. 9, pp. 519-530, 2014, DOI: 10.1007/978-94-007-7811-5_48, ISBN: 978-94-007-7811-5.
This law has an unsymmetrical behaviour.
|
|
|
Data requested for an Unsymmetrical Slip-type behaviour are:
§ Kel: elastic stiffness assigned to the spring;
§ Fy: strength at elastic limit;
§ Kpl1: slope of the positive plastic branch, must be ≠0;
§ Fmax: maximum strength reachable;
§ Kpl2: slope of the negative plastic branch, must be ≠0;
§ cKunload: it sets the unloading stiffness of the first branch of unloading (green) and of reloading (blue) path by multiplying the elastic stiffness by this factor;
§ cFreload: it sets the lower limit of last branch of reloading (blue) and unloading (green) path, in percentage of the force value in the backbone. Such parameter must be set between 0 and 1;
§ cFunload: it sets the lower limit of first branch of unloading (green) and reloading (blue) path, in percentage of the force value in the backbone. Such parameter must be set between 0 and 1;
§ Uu: ultimate displacement allowed;
§ Fmin: maximum strength reachable in compression;
§ Kneg: stiffness coefficient for compression branch, multiplies the elastic stiffness;
§ cFend: coefficient for setting the force value at the end of the last branch of the unloading path (green), multiplies the yielding force;
§ cFinit: coefficient for setting the force value at the beginning of the first branch of the reloading path (blue), multiplies the yielding force;
§ alpha: exponential strength degradation parameter based on dissipated energy;
§ beta: exponential strength degradation parameter based on maximum displacement reached;
§ gamma: linear strength degradation parameter;
§ cKreload: sets the unloading stiffness of last branch of the reloading (blue) and unloading (green) path by multiplying the elastic stiffness by this factor.
- Dashpot: represents a non-linear damper element accordingly to Kelvin’s model. This law is suitable for dynamic analysis, and gives a response defined as:
where the stiffness is
The needed parameters are:
§ Kr: restoring stiffness of the dashpot;
§ C: damping coefficient;
§ a: damping exponent;
§ K0: initial stiffness of the dashpot;
§ F0: preloading force. Below this value, damper is not active.
- AMD: represents a linear damper (except for Fmax, Vmax, and Dmax limits) as per Maxwell model (damper and spring in series). If Fmax is non-zero, the damper limits the supplied force by behaving elastically-perfectly plastic. Vmax and Dmax can be used to represent an Active Mass Damper with limits in velocity and displacement. Required parameters are:
§ K: damper stiffness
§ G: damping coefficient
§ a: damping exponent;
§ Fmax: maximum force for the damper
§ Dmax: maximum displacement of moving mass
§ Vmax: maximum velocity of moving mass
State variables are available for this element, which can be consulted in Extract data mask, under 'Stations/Points'. They contain, in order:
§ s1: speed at i-th step
§ s2: force at pitch
§ s3: energy dissipated by the damper
§ s4: acceleration rel. mass
§ s5: mass-related velocity
§ s6: displacement rel. mass.
- VRM: simulates a broad class of complex hysteresis loops as described in Vaiana N, Rosati L (2023) Classification and unified phenomenological modeling of complex uniaxial rate-independent hysteretic responses. Mech Syst Sig Process 182: 109539 and in Vaiana N, Rosati L (2023) Analytical and differential reformulations of the Vaiana-Rosati model for complex rate-independent mechanical hysteresis phenomena. Mech Syst Sig Process 199: 110448.
The data required by the Vaiana Rosati model are:
· kb+: angular coefficient of the upper boundary line 
(Fig. a)
· f0+: ordinate of the point 
(Fig. a)
· alpha+: parameter that adjusts the curvature of the load curve 
(Fig. a)
· beta1+: parameter that transforms into a curve without an inflection point by adjusting its curvature (Fig. b)
· beta2+: parameter that transforms into a curve without an inflection point by adjusting its curvature (Fig. b)
· gamma1+: parameter that transforms into a curve with inflection point by adjusting the distance between 
and 
(Fig. c)
· gamma2+: parameter that transforms into a curve with inflection point by adjusting the slope of 
(Fig. c)
· gamma3+: abscissa of the inflection point (Fig. c)
· umax: positive ultimate displacement
· All previous parameters followed by "-": the same properties for the unloading phase
· umin: negative ultimate displacement.
WARNING: for the use in OpenSees of non-linear springs, see www.nextfem.it/it/opensees/ to install the OpenSees solver. Also set the desired options in the boxes in the Options mask, tab Misc.
