Pressures Panel

Use the Pressures panel to create pressure loads on elements by applying a load, representing pressures, to a 1D or 2D element, or to the face of a solid element.

Location: Analysis page

For most solvers, the pressure load is considered as force/area, therefore the magnitude of the pressure is multiplied by the calculated area of the elements to which it is applied and resolved as concentrated force loads at the associated nodes.

Pressures are load config 4 and are displayed as a vector with the letter P at the tail end.

Create Subpanel

Use the Create subpanel to create new pressures. You can specify the pressure's footprint by selecting the elements it affects, as well as its direction, magnitude, and the size in which its visual indicators are drawn. You can also apply the pressure to the faces of solid elements, or to the edges of plate elements.

For plate elements, the pressure is applied along the positive element normal. The Normals panel should be used first to obtain the correct orientation. The nodes on face option is not necessary if applying the pressure to the face of a plate element. If applying the pressure to the edge of plate elements, the nodes on edge option is required to define which of the three or four edges of the plate element you wish to apply the pressure to. For solid elements, the nodes on face option is required to define which of the faces you wish to apply the pressure to.

Option	Action
elems selector	Select elements (1D, 2D, 3D) to which pressures will be applied. Use the switch to change the selection mode. elems Select individual elements, or select all of the elements contained by a component or on a surface. Figure 1. Example: Elems Selection faces Select all of the elements on 2D and 3D faces. If there are discontinuities on a 2D face, then only the elements in between the discontinuities will be selected. Figure 2. Example: Faces Selection 2D faces ext Select all of the elements on a 2D face that contain discontinuities. Figure 3. Example: 2D Faces Ext Selection free edges Select all of the free edges of elements. If there are discontinuities on an edge, then only the free edges of elements inbetween the discontinuities will be selected. Important: Only valid for SHELL elements. Figure 4. Example: Free Edges Selection free edges ext Select all of the free edges of elements that contain discontinuities. Important: Only valid for SHELL elements. Figure 5. Example: Free Edges Ext Selection loops Select all of the continuous free edges of elements that make a closed loop simultaneously, such as the perimeter of a hole. Important: Only valid for SHELL elements. Figure 6. Example: Loops Selection Note: If you leave the Pressures panel, your current selection will disappear, but it will be restored once you return to the panel. Changing the selection mode will clear your current selection. Use the Entity Editor to select elements using multiple selection modes.
magnitude =	constant vector Specify the magnitude, then use the plane and vector selector to specify the vector along which the load should act. constant components Specify the direction and magnitude of the load by entering the X, Y, and Z values of the components. curve, vector When working with loads that are time dependent, use this method to first specify a magnitude (yscale) for the curve. Next, double-click curve to select an existing curve, then use the plane and vector selector to specify a direction, if necessary. Last, specify a factor for the curve's xscale to use the same curve for many different cases, but vary the scale of its intensity or time to match the needs of your current moment. curve, components Specify the X, Y, and Z components to define the direction and magnitude, for example, (2,2,2) will be twice the magnitude of (1,1,1). Next, double-click curve to select an existing curve. Last, specify a factor for the curve’s xscale to use the same curve for many different cases, but vary the scale of its intensity or time to match the needs of your current load. equation Specify the loading equation.^¹ Use the plane and vector selector to specify a direction, then select the coordinate system to which the vector corresponds. linear interpolation Interpolate loads from a saved file or existing loads. Note: Only available for shell elements. Each row of the input file contains the x,y,z coordinates of the load followed by its three components. The data can be separated by a space or tab. You can then select the desired nodes to which you wish to add loads, and pick 3 or more existing loads that enclose those nodes. When you interpolate, a linear function is used to create additional loads on the selected nodes, with magnitudes based on the magnitudes of the loads that you had selected. Figure 7. In the search radius field, specify the search distance to find the loads which are within that distance from a centroid or node on which a load is being interpolated. The nearest 3 loads located within that distance are used to create the load at the centroid or node by linear interpolation. Linear interpolation uses a triangulation method, so if it finds fewer than 3 loads within that distance no interpolation takes place. While reading the initial loads from a file, if linear interpolation is not possible because the search radius is too small, the original loads are simply applied to the nearest centroid or node. Select fill gap to create a load at every selected element centroid or node irrespective of the size of the search radius. field loads Interpolate and extrapolate loads from existing loads. You can then select the desired elements to which you wish to add loads, and any existing loads on which you wish to base additional forces. When you create, HyperLife Weld Certification uses a Green's function with the given boundary loads in order to create the loads on all of the selected nodes. For smoothness, the gradient at the boundary points is enforced to be zero; this ensures that the extrapolated loads remain lower than the input loads. For this reason it is recommended to use representative boundary values as input to be able to capture the peaks reasonably. Note: This version differs from linear interpolation both in the way that the load magnitudes are determined, and also in the fact that it can be applied to nodes outside the boundaries of the chosen existing loads.
normal / N1,N2,N3	normal Created pressure will be in the positive normal direction as determined by the normals of the chosen elements N1,N2,N3 Select three nodes to define a plane; the pressure is applied in the positive normal direction of that plane as determined via the right-hand rule.
relative size / uniform size	relative size Display pressures in a size relative to the model size (default 100). By default, pressures are displayed relative to the model size. uniform size Display all pressures with the same size. Note: This setting does not affect the pressure load, only the length of its graphical indicators.
label loads	Display text labels for each of the loads in the modeling window.
nodes on face / nodes on edge	nodes on face Apply pressures to the face of a solid element. The face or edge nodes define the starting face or edge. For a four-noded face, select the diagonally opposing nodes. For a three-noded face, select all of the nodes. You can select a surface that represents the faces you want the loads to be applied to. This places loads on the faces of all elements associated with the selected surface. Alternatively, select the nodes representing the face of the solid element the load is to be applied to. nodes on edge Apply pressures to the edge of an element for an axisymmetric problem. You can select the nodes that represent the edge of the element you want the load on, or the lines that represent the edges of all the elements that you want to place loads on. Note: Available when the selector is set to entities.
face angle / individual selection	face angle Determines which of the selected support entities will have the panel entity (ex: load, boundary condition, vector, set definition, and so on) applied. The face angle value is used to determine which faces will be selected based on the angle difference between the selected and adjacent face normals. If the angle between the normals of the faces is less than this face angle value the face is included. This process is similar for edge selection, except that the angle between edges is used instead of the angle between faces. Important: Only available when the entity selector is set to nodes, and the selection mode is set to faces, 2d faces ext, free edges, free edges ext, edges, or edges ext. individual selection Select individual elements on a face or select individual free/shared edges of elements. Important: Only available when the entity selector is set to nodes and the selection mode is set to faces, free edges, or edges.
edge angle	Split edges that belong to a given face. When the edge angle is 180 degrees, edges are the continuous boundaries of faces. For smaller values, these same boundary edges are split wherever the angle between segments exceeds the specified value. A segment is the edge of a single element. Important: Only available when the entity selector is set to nodes and the selection mode is set to free edges, free edges ext, edges, or edges ext.
load types =	Select a load type to apply to the pressure.

Update Subpanel

Use the Update subpanel to alter existing pressure loads. You can select the desired loads and edit their magnitude, direction, visual indicator draw size, and load type.

Option	Action
loads	Select the existing loads that you wish to modify.
display	Display the loads on the model.
magnitude =	constant vector Specify the magnitude, then use the plane and vector selector to specify the vector along which the load should act. constant components Specify the direction and magnitude of the load by entering the X, Y, and Z values of the components. curve, vector When working with loads that are time dependent, use this method to first specify a magnitude (yscale) for the curve. Next, double-click curve to select an existing curve, then use the plane and vector selector to specify a direction, if necessary. Last, specify a factor for the curve's xscale to use the same curve for many different cases, but vary the scale of its intensity or time to match the needs of your current moment. curve, components Specify the X, Y, and Z components to define the direction and magnitude, for example, (2,2,2) will be twice the magnitude of (1,1,1). Next, double-click curve to select an existing curve. Last, specify a factor for the curve’s xscale to use the same curve for many different cases, but vary the scale of its intensity or time to match the needs of your current load. equation Specify the loading equation.^¹ Use the plane and vector selector to specify a direction, then select the coordinate system to which the vector corresponds. linear interpolation Interpolate loads from a saved file or existing loads. Note: Only available for shell elements. Each row of the input file contains the x,y,z coordinates of the load followed by its three components. The data can be separated by a space or tab. You can then select the desired nodes to which you wish to add loads, and pick 3 or more existing loads that enclose those nodes. When you interpolate, a linear function is used to create additional loads on the selected nodes, with magnitudes based on the magnitudes of the loads that you had selected. Figure 8. In the search radius field, specify the search distance to find the loads which are within that distance from a centroid or node on which a load is being interpolated. The nearest 3 loads located within that distance are used to create the load at the centroid or node by linear interpolation. Linear interpolation uses a triangulation method, so if it finds fewer than 3 loads within that distance no interpolation takes place. While reading the initial loads from a file, if linear interpolation is not possible because the search radius is too small, the original loads are simply applied to the nearest centroid or node. Select fill gap to create a load at every selected element centroid or node irrespective of the size of the search radius. field loads Interpolate and extrapolate loads from existing loads. You can then select the desired elements to which you wish to add loads, and any existing loads on which you wish to base additional forces. When you create, HyperLife Weld Certification uses a Green's function with the given boundary loads in order to create the loads on all of the selected nodes. For smoothness, the gradient at the boundary points is enforced to be zero; this ensures that the extrapolated loads remain lower than the input loads. For this reason it is recommended to use representative boundary values as input to be able to capture the peaks reasonably. Note: This version differs from linear interpolation both in the way that the load magnitudes are determined, and also in the fact that it can be applied to nodes outside the boundaries of the chosen existing loads.
normal / N1,N2,N3	normal Created pressure will be in the positive normal direction as determined by the normals of the chosen elements N1,N2,N3 Select three nodes to define a plane; the pressure is applied in the positive normal direction of that plane as determined via the right-hand rule.
relative size / uniform size	relative size Display pressures in a size relative to the model size (default 100). By default, pressures are displayed relative to the model size. uniform size Display all pressures with the same size. Note: This setting does not affect the pressure load, only the length of its graphical indicators.
label loads	Display text labels for each of the loads in the modeling window.
load types =	Select a load type to apply to the pressure.

Command Buttons

Button	Action
create	Create a new pressure on the selected elements, based on the criteria you have specified.
create/edit	Create a new pressure on the selected elements, based on the criteria you have specified, and open a temporary card editor panel based on the specified load type.
reject	Undo the most recent create action.
update	Change the selected pressure to have the characteristics currently set in the Update subpanel.
review	Click review, then select a pressure in the modeling window to display the characteristics for that load (such as magnitude, vector, X/Y/Z/ components, and so on) in the panel fields.

Equations allow you to create force, moment, pressure, temperature or flux loads on your model where the magnitude of the load is a function of the coordinates of the entity to which it is applied. An example of such a load might be an applied temperature whose intensity dissipates as a function of distance from the application point, or a pressure on a container walls due to the level of a fluid inside.

Functions must be of the form magnitude= f(x,y,z). The only variables allowed are x, y and z, (lower case) which are substituted with the coordinate values of the entity to which the load is applied. In the case of grid point loads (force, moment or temperature) the grid point coordinates are used. For elemental loads (pressure or flux) the element centroid coordinates are used. In the event that a cylindrical or spherical coordinate system is used, x, y and z are still used to reference the corresponding direction. Standard mathematical operators and functions can be used; however, any functions requiring external data will not be valid.

Note: If your equation contains a syntax error, no warning message will be displayed, but any loads created will have a zero magnitude.