Featured Case StudyThe Norsea Gas Terminal in Northern Germany plays a vital role in the connection of pipeline systems coming from the North Sea to the natural gas distribution network throughout Germany. Built in...Stay
- ANSYS Software
Featured Case StudyRelying on ANSYS Composite PrepPost helped EADS Innovation Works to develop lightweight composites in aircraft design. ANSYS Composite PrepPost provided simple pre- and post-processing of composite...Stay
- Resource Library
- News &
Caution: Contacts Under Pressure!
Have you ever had to model a bolted interface on an assembly with an internal pressure? Consider a simple example, shown in Figure 1 above, of a bolted pipe connection under internal pressure. The goal is to maintain a seal between the pipe flanges and keep the connection from leaking. To accomplish this, a bolt pre-load is applied, prior to the pressure, that pushes the surfaces of the flanges together.
Contact elements are used to keep the pipe flange surfaces from penetrating. The location of the contact region between the flanges is shown in Figure 2.
Figure 2 - Frictional Contact Region Between the Pipe Flanges
When the pressure is applied to the inner walls, it may pry open the connection at the flanges. This is illustrated in the exaggerated plot of the radial deformation in Figure 3.
Figure 3 – Radial Deformation of the Pipe Section Under Internal Pressure
To maintain a seal, you will need sufficient preload in the bolts, and the contact element results can help you determine this. In addition, the contact status and gap can help you identify the optimum location to add an o-ring, if needed. For this example, the status of the contact between the flanges is shown in a plot of the expanded structure Figure 4. Note that the continuous red band of closed status in the tangential direction indicates that no leakage should occur.
Figure 4 – Contact Status at the Flange Connection
However, the results above do not take into account that the exposed surfaces in the gap should have pressure applied to them when they come out of contact. This can be difficult to accomplish for the following reasons:
1. The area of the open contact is not initially known.
2. The contact status continuously changes as the pressure is ramped on.
The good news is that some finite element programs, such as ANSYS, allow you to apply the pressure directly on the faces of the contact elements. Contact elements with a closed status ignore the applied pressure. The pressure is activated when the contact element status changes to open. The pressure field will update at each load increment as the contact status is evaluated. The effect is that the pressure is allowed to move into the gap as it opens.
This provides a more realistic evaluation of the design. To illustrate, the contact status of the same model with and without pressure included in the gap is shown in Figure 5. Note that the added pressure creates an open path between the bolts, indicating that leakage will occur. Clearly, more bolt pre-load or perhaps more bolts are needed to maintain a seal.
Figure 5 - Effect of Adding Gap Pressure on the Contact Status
So what is the approach for applying pressure directly to the contact elements? The first step is to determine if your finite element program supports fluid pressure penetration loading. If that is the case, it is also critical that you define contact elements on both sides of the interface using a symmetric contact generation. Using asymmetric contact will only add the pressure on one side.
In ANSYS, you can select the contact elements and apply the pressure to them directly if you are using the MAPDL interface. In ANSYS Mechanical, the contact surfaces can be promoted to surface Named Selections.The surface Named Selections will be converted to nodal components during the solution phase so a command block with some MAPDL command logic will be needed. A sample command block is shown in Figure 6.
Figure 6 - ANSYS Mechanical Command Block
I think we can all agree that it’s better to repair a leaky pipe during the design phase of a project rather than in the field. I hope this post helps keep you safe and dry.
by: Patrick Cunningham
by: Peter Barrett
by: Jonathan Dudley
by: Peter Barrett
by: Michael Bak
- Engineering Consulting
- ANSYS Software & Support
- ANSYS Training
- About Us
- News & Insights
1579 Straits Turnpike Suite 2B
Middlebury, CT 06762
- ANSYS Software