Pressure-penetration loads can simulate surrounding fluid or air penetrating into the contact interface, based on the contact status. You can apply pressure-penetration loads to flexible-to-flexible or rigid-to-flexible contact pairs. 2-D and 3-D surface-to-surface contact elements (CONTA171, CONTA172, CONTA173, CONTA174) support pressure-penetration loading.
Fluid pressure can penetrate into the contact interface from one or multiple locations. The fluid pressure-penetration load has a path dependent nature. The penetrating path can propagate and vary, and it will be determined iteratively. At the beginning of each iteration, ANSYS first detects starting points which are exposed to the fluid pressure. Among the starting points, ANSYS then finds fluid penetrating points where the contact status is open or lost, or where the contact pressure is smaller than the user defined pressure-penetration criterion. When a contact detection point has a contact condition of “penetrating,” it is subjected to the fluid pressure, and its nearest neighboring nodes are considered to be the starting points which are exposed to the fluid pressure as well.
The fluid pressure will not be applied to an area having a contact status of open unless the edges/ends of the area belong to the starting points.
The fluid pressure starts to penetrate into the interface between contact and target surfaces from the penetrating points. The fluid penetration can be cut off when contact between the surfaces is reestablished or when contact pressure is larger than the fluid penetration criterion.
To model fluid penetration loads, you need to specify the following quantities:
An example analysis showing how to apply fluid penetrating loading is presented in Appendix A.
The fluid pressure must be applied to contact and target elements using the SFE command:
The pressure is applied only on the corner nodes of the contact and target elements. The pressure on the midside nodes of CONTA172, CONTA174, TARGE169, and TARGE170 will be averaged using the pressures of two adjacent corner nodes. VAL3 and VAL4 are not used for 2-D contact and target elements.
Pressure value VALi, which is applied to the ith node (where i = 1, 2, 3, 4 indicates node I, J, K, L, respectively) of the contact or target element, can be a constant numerical value or a table name. If it is constant, the magnitude of pressure will be step-applied or ramped based on the KBC command setting. To specify a table, enclose the table name in percent signs (for example, %tabname%). Use the *DIM command to define the table. Only one table can be specified, and it must be specified in the VAL1 position; tables specified in the VAL2, VAL3, and VAL4 positions will be ignored.
The fluid pressure-penetration load will be automatically applied to the penetrating points on contact and target surfaces based on the contact status.
By default (KEYOPT(14) = 0 on the contact element), the fluid pressure-penetration load varies during iterations based on the current contact status. In certain cases, the default can cause an unstable convergence pattern since the contact status and the resulting applied fluid penetration load keep changing during iterations.
When KEYOPT(14) = 1, the fluid pressure-penetration load will be applied to the contact and target elements at the beginning of each substep and will remain constant over that substep even if the contact status keeps changing during iterations. Small increments are often needed to obtain accurate results.
Keep the following points in mind when defining fluid penetration loads:
For flexible-to-flexible contact with a symmetric contact pair definition (including a self-contact pair), you should apply the fluid pressure only to the contact elements.
For flexible-to-flexible contact with an asymmetric contact pair definition, you should generally apply fluid pressure on both contact and target elements which are currently or will potentially be exposed to the surrounding fluid. ANSYS will ignore fluid penetration loads applied to a target surface if there are no fluid penetration loads applied to the associated contact surface within the contact pair. When the fluid pressures are applied to both contact and target elements, ANSYS will have to identify the penetration paths for both the contact surface and the target surface. The iterative process of determining the penetration path on the target surface is very time-consuming, particularly for 3-D contact models. Therefore, we strongly recommend that you use a symmetric contact pair definition since it does not require the specification of fluid penetration pressure on the target surface.
For rigid-to-flexible contact, you should apply the fluid pressure only to the contact elements. ANSYS will automatically apply equivalent forces to the rigid target surface to balance out the applied pressure on the contact surface. Fluid pressure applied to the rigid target surface will be ignored.
For situations in which multiple contact pairs are defined on the same surface, contact elements may overlap each other. In this case, be careful to apply the fluid penetration pressure only once in areas where contact elements overlap.
The fluid penetration pressure can only be applied to the contact and target elements using the SFE command. Other pressure load commands (SF, SFL, SFA) can not be used. In addition, you should not apply the pressure on the underlying elements.
ANSYS ignores any fluid penetration pressures applied to MPC based contact pairs.
The effects of pressure load stiffness are automatically included. If an unsymmetric matrix is needed to achieve convergence for pressure load stiffness effects, issue the NROPT,UNSYM command.
When a fluid pressure-penetration load is applied, the fluid pressure penetrates to the surface from defined starting points. There can be one or multiple starting points. ANSYS will automatically find the default starting points by selecting free end points of 2-D contact/target surfaces or nodes of free open edges on 3-D contact/target surfaces ("free" meaning that the element is not fully surrounded by adjacent elements; see figure below).
The starting points are initially exposed to the fluid and are potentially subjected to the penetration pressure. There are no default starting points if the contact or target surface is continuous with a closed loop. The default starting points can be overwritten using the SFE command. You can specify starting points, specify penetrating points, and remove the default starting points with the SFE command and STAi values, as described below. Be sure to set LKEY = 2 on the SFE command in order to specify the STAi settings. The command format is:
|STAi = 0 (default)||ANSYS determines whether the ith node is a starting point based on the contact status. The ith node can be a default starting point if the node is a 2-D free point or is on a 3-D free edge.|
|STAi = 1||The ith node is the starting point which is initially exposed to the fluid. It can be a penetrating point if the initial contact status is "open." The node may no-longer be the starting point when the contact status changes during the deformation process.|
|STAi = 2||The ith node is a penetrating point. The node is always subjected to the fluid pressure in spite of any contact status change.|
|STAi = -1||The ith node will not be a default starting point even though it belongs to a 2-D free point or a 3-D free edge node.|
If only STA1 is specified and the other STAi values are blank, STA2, STA3, and STA4 will default to STA1.
You can specify a pressure-penetration criterion using the contact element real constant PPCN. When the contact pressure is less than the criterion, the starting point turns into the penetrating point; that is, fluid pressure starts to penetrate. Thus, a higher criterion value will allow the fluid to penetrate more easily. When the contact pressure is greater than the criterion, the penetrating point returns back to the starting point; that is, fluid penetration is cut off. By default, the penetration criterion (PPCN) is zero. In this case the fluid penetration occurs only when the contact is open, and the cutoff of fluid penetration occurs only when the contact is reestablished.
You can input PPCN as a constant value or as a table of values. The tabular input can be a function of contact point current location (global X , Y, Z), contact pressure, time, or temperature. To input a table name, you must enclose the name in % symbols (for example, %tabnam%). Use the *DIM command to define the table.
When the fluid pressure penetration occurs, the fluid pressure is applied normal to the contact/target surfaces. As with conventional pressure loading, the current amount of fluid pressure at a given substep will depend on whether the pressure is input as a constant value or a table of values, and whether the pressure is ramp- or step-applied (KBC command). If the total amount of fluid pressure is applied instantaneously, convergence difficulties may arise due to large changes in stresses near the contact interface. This is also true when the fluid penetration pressure is removed instantaneously, as when the fluid penetration is cut off. To help stabilize the solution, ANSYS offers an option to ramp the fluid pressure linearly over a time period, during one or several substeps.
To implement this ramping option, specify the fluid penetration acting time using the contact element real constant FPAT. Input a positive number to define the fraction of the time increment of the load step; input a negative number to define the absolute acting time. The default penetration acting time is 0.01 times the time increment of the current load step.
At each penetrating point, if the time increment of the current substep is less than the fluid penetration acting time (FPAT > (tn - tn-1)), the fluid pressure is ramped up linearly from the actual applied pressure of the previous substep to the full current amount of the fluid pressure over the penetration acting time period; otherwise (FPAT ≤ (tn - tn-1)), the full amount of current fluid pressure will be applied. (See figures below.) At the pressure-penetration cutoff points, if the time increment of the current substep is less than the fluid penetration acting time, the fluid pressure is ramped down linearly from the applied pressure of the previous substep to a zero magnitude over the penetration acting time period; otherwise, the fluid pressure will be immediately removed.
You can redefine or modify fluid pressure-penetration loads and fluid penetration starting points between load steps using the SFE command.
You can also modify the pressure-penetration criterion (real constant PPCN) and acting time (real constant FPAT) using the RMODIF command.
To remove a fluid pressure-penetration load, use one of the following methods:
Because these methods remove the fluid penetration pressure immediately, convergence difficulties may occur. To avoid this problem you can add an extra load step which applies a small fluid pressure (for example, VALi = 1e-8) via the SFE command instead of removing the pressure.
You can list and display the actual fluid penetration pressure applied on contact and target elements using FPRS as a contact result item on the PLNSOL, PLESOL, PRNSOL, and PRESOL commands. For example:
You can also list and display the fluid penetration pressure applied on target elements by using the ETABLE command.