Paulin Research Group Houston, Texas

Meshing Plate Supports

Meshing plate supports is one of the most complicated tasks in FE/Pipe, but once dominated, a lot of things can be modeled. We are going to model a simple support that will demonstrate how to properly mesh the plate support using the Parent Surface Control.

FE/Pipe usually does not align the mesh for plate supports. This is due to the fact that the mesh density has to be input by the user, therefore, if all meshing parameters are left blank, then default number of nodes for plates will not match the default number of nodes of the shell.

Select the template General Nozzles, Plates and Shells.

Enter the geometry of the shell under Shell Geometry. In this case “Cylinder” will be used, and a length of 400in.

The next steps are to create plates. There is a certain procedure that has to be done in order to make the process simpler to understand.

First, the plate points need to be located with respect to the parent geometry, in this case CYLINDER. The FE/Pipe Manual Chapter 2, Section 8, shows how to model plates.

There are different ways to locate points, by (C)enter, which will start locating the points from the centerline of the header. (S)urface, that will start from the surface of the cylindrical shell. (A)bsolute which will start from the 0, 0, 0 position of the header and (D)elta, which will only mean a change in the Cartesian Co-ordinate system. Whether the user defines (S) or (C), the point along the surface of the shell or the point along the centerline of the vessel, is defined by the user in “Location” in Plate Geometry. The angle in which the plate will start is also defined by the user under “Orientation” in Plate Geometry main screen.

The table below shows the point locations for all 6 points of the plate. Plates only require 4 points, but having 6 points can improve the meshing. When curvatures are small, then having more points will produce a much better mesh, as well as increasing the number of elements in the plate.

Point ID	Point Status	R Coordinate	S Coordinate	T Coordinate
1	1	-100	0	0
2	1	0	0	0
3	1	100	0	0
4	3	-100	12	0
5	3	0	12	0
6	3	100	12	0

All points are defined from the Surface of the parent geometry. The start location, as mentioned earlier will be defined under Plate Geometry.

After defining the plate points, we can create the plate geometry. We are going to define the plate, by specifying which points will be at the surface and which points will be away from the surface. Also, we will determine which point connects are to be connected together. This is critical in the modeling of plates, if the order of the points is flipped, then the plate will not plot correctly.

The near point list will be defined by the points that are at the surface of the cylindrical shell. The far points are the ones removed from the surface. The order of these points will determine how the model is meshed by Modgen (Graphical window of FE/Pipe). The near edge type is defined as “0” and “2”, the former stands for attached to the parent geometry and the latter stands for straight edge.

After the longitudinal plate is defined, we can go back to Plate Geometry and specify what is required to plot the plate. Below is the main screen of the Plate Geometry. In here we define the starting point on which the coordinate system is to start. The orientation angle is set to 180 degrees, and the location is the center point of the cylinder, at 200in. The orientation angle can be set to zero if the Zero Degree Orientation under General is set to –Y (0, -1, 0). Right now it is set to +Y (0, 1, 0) and the Centerline Axis Orientation set to +X (1, 0, 0). Make sure to change the “Use Alt Meshing?” to YES.

Alt Meshing will allow the user to control the meshing of the plate and the header more freely.

The next step is to add boundary condition to the header. Under Shell Boundary Conditions, we can set the TOP of the cylinder to be FIXED and the BOTTOM to be PFIX. PFIX will allow longitudinal displacement for proper Pd/4t computation of stress.

Then material properties and pressure should be applied to the shell.

Then enter the material properties of the plate. The Plate or Nozzle number must match the Plate ID placed in the Plate Geometry Window.

The model is now ready to plot. The screen below shows the default plot of the model. If you select End View from Viewing, you will see that the alignment of the meshing of the shell does not match the plate support.

To make the meshing match for any plate support, radial mesh breakdown should be added at the end of the plate support on the shell. To do this, in the Optional Window, Radial mesh breakdown should be entered at the two locations (i.e. 100 and 300in). After doing this and plotting, you will be able to see the rings by clicking on Settings, then Stamps and then Rings.

Another set of radial mesh breakdown should be added at SQRT (RT). Within this distance from a discontinuity, the stresses are considered to be local stress and go under the ASME Section VIII Div 2 code as P_l. In this case, SQRT (RT) will be 3.7in.

Knowing the amount of rings the model has is very important when trying to mesh plates. In this model there are 2 user defined rings, and 2 software-defined. FE/Pipe placed a ring at 200in because there are two nodes defined by the user at this location; nodes 2 and 5 are at the center of the parent shell. So the user defined rings are from 96-100, from 300-304, Then the software will create two extra rings, from 100-200 and from 200-300. The number of elements within each ring can be modified by the user to have more elements on a certain part of the model, higher density mesh usually means more accurate results.

Under Optional, there is a button called Global User Surface Control. This is the window used to control the mesh for the cylinder.

In this window, the user can select to control all the rings and angles in the model. In this case, what needs to be done is to control the rings in the center of the model, above the plate and within SQRT (RT). It is important to have at least two elements within this area. To place elements within the rings, Element Number needs to be chosen.

The first ring needs to have 3 elements, therefore for the first user defined ring; we place a 1 and the number of elements (3).

We keep adding pages, and for the next user defined ring, we need to place the largest amount of elements, as it is the biggest distance within rings. We need to do this for rings 2 and 3.

Finally for the fourth ring we can add 3 more elements.

Then Press E-Plot. You will see that the meshing on the surface is dense enough for good results. Now the plate mesh density needs to be changed. This can be done in the Plate Geometry window, under Longitudinal Plates. I placed 21 for both sides of the plate created and 5 nodes going along the radial direction for better mesh. There is an option to change on the right hand side called “Fine Mesh at:”, if NEAR is selected there will be a finer mesh closer to the near side of the plate, that is closer to the shell. This is what is best as closer to the discontinuities we need more elements for more accurate results.

Then plot should look like the picture below.

We can see that in the parts where we have discontinuities, we have denser meshing.

For time saving purposes, the mesh should only be dense near the plate, for this we can create or eliminate angles created automatically by the software so that the denser mesh will be near the plate. The angles FE/Pipe creates by default are shown below.

Global User Surface Control can be used to eliminate or create extra angles. What these angles do is to define the meshing parameters within these angles in the radial direction. We do not need so many angles at the top of the pipe as this is not the most important part to be analyzed, so we are going to erase some of these, and leave the important ones, near the support. In the main window of Global User Surface Control, select “User Control of ALL Angles” from NO to YES. The user will now control all of the angles in the model. In the picture below you can see that the bottom part of the pipe, closer to the support has more angles defined.

Angles at 45 degrees apart were placed for denser mesh closer to the support.

Then, in the same page that Rings were created, under Element number, this time ANGLES are going to be created. Counting the same way as rings were counted, angles 3 and 4 are the ones closest to the plate.

Pressing E-Plot you will see the following.

The meshing on the bottom of the model is much denser, but the top is less dense, therefore saving some running time. You can reduce even further the top part, by adding angles and placing very few elements within these regions.

The model is ready to run. Press I-Submit and Wait.

We can see clearly the pressure effects on the pipe and how the support reacts to the deforming of the pipe.