Paulin Research Group Houston Texas

Trunnion with an End Cap and Lug

Difficulty level: Intermediate to Advanced

Topics:

· Advanced Database Operations (join by proximity)

· Generalized Structural Shapes

The objective of this technical note is to demonstrate techniques that can be used to model a support trunnion with a structural attachment. This type of construction is sometimes used to attach snubbers and sway braces to piping.

Overview:

This model is constructed by combining two separate models using an advanced “Database” operation. A “database” operation is a mechanism within FE/Pipe to build complex geometric models from simple component models. A general procedure for using database operations is included at the end of this tutorial.

In this example, the two models will use the “join by proximity” method of database operations. This is an advanced method of Database operations.

The first model is of the pipe and trunnion with a circular reinforcement pad. This sub model may be built using one of two templates in FE/Pipe:

(i) The general nozzles plates and shells template (“Nozshel”), and

(ii) The pad-reinforced fabricated tee template (“RFT”).

Using the Nozshel template provides the most flexibility, but imposes the greatest complexity. This example will use the RFT template because of its simplicity. Be cautious: the RFT template can not apply loads in the “header” piping. Therefore, the Nozshel template should be used if the loads (stresses) in the piping are significant.

The second model is a generalized structural shape built using the Nozshel template. The structure is constructed using “plates”. Detailed information on plate construction is available in Chapter 2 Section 8 of the FE/Pipe user’s manual (accessed from the FE/Pipe startup window as shown below)

Part 1 - Building Model 1

Step 1. Create a new file select “pad-reinforced fabricated tee”

Step 2. Setup the model coordinate system.

Usually model loads are determined using a pipe stress analysis program. The simplest way to ensure that loads are applied correctly is to align the finite element model to the same coordinate system as the pipe stress model.

Open the “2-General” screen and input the orientation cosines.

Step 3. Input the branch diameter and wall thickness.

Open the “3-Branch Properties” screen and input the data below. For code compliance reports, also input the allowable stresses in this screen. Do not input pressure on this screen because the pressure in the trunnion is at atmospheric pressure.

Step 4. Input the pipe diameter & wall thickness and pad dimensions

Open the “5-Header/Vessel/Pad Properties” screen and input the data shown below. Input the operating pressure on this screen.

Step 5. Input the weld sizes

Open the “6-Weld Details” screen and input the weld data below. If no weld size is specified, FE/Pipe will assume an arbitrary fraction of the header and branch wall thickness. This screen may also be used to control the fatigue performance and mesh density in the weld elements.

Step 6. Specify pipe lengths and some miscellaneous model parameters

Open the “9-Optional” screen and input the attached pipe lengths.

Change the “relative stiffness (to branch) of loading ring” to 1 from 10000. The default value of 10000 is used to restrict ovalization when loads are applied to the branch end

Mesh controls are also included in this screen, and may be modified to the designers’ satisfaction. Only one other default setting is changed in this example; that is “Compute stress in Weld elements”. This change is optional and should be used with caution. The isoparametric shell elements only have two integration points through the thickness and do not provide good estimates of through thickness stress (shear) distributions.

Step 7. Setup the Database Operations

Open the “A-Database Operations” screen. Change the database read/write option to “1” (export).

Step 8. Select “E-Prepare for Analysis”.

Completed Construction of Model 1

Part 2 - Building Model 2

Step 1. Plan the geometry layout.

Best results will be obtained when the surface boundaries of the “plates” match with the midsurfaces of the trunnion model. The surface boundaries of the branch can be determined from a plot of trun01.ifu by following the sequence of figures below.

(Click ok)

The surfaces can be examined more closely using the “viewing” => “rotate/pan/zoom” tool. It will be seen that there are 8 evenly spaced surface divisions about the branch circumference, giving regular angular divisions of 45 degrees.

“Plate Points” are required to define the corners of each of the surfaces (i.e. the intersection of each of the green lines above).

Step 2. Create a new File

Select “General Nozzles Plates and Shells” template

Step 3. Set the model type as “none” to define a generalized structure

Select the “3-Shell Geometry” screen and input the data below. A diameter and wall thickness is still required because the template uses this data to estimate the “merge nodes tolerance”

Step 4. Define a Plate assembly

Select the “7-Plate Geometry” screen and input the following data. A “plate number” defines an ID for the collection of circumferential, longitudinal and other individual plates.

In this unusual case, it is not important what values are specified for “orientation angle” and “location”… so long as at least one of these values is non-zero.

Step 5. Define the “plate points”

From within the “7-Plate Geometry” screen, click the “plate points [F7]” button. Type in the coordinates for all the points based on the desired geometry (sample coordinates shown below).

Note the following graphic of the plate point screen. There are two important factors:

(i) All points for a general structure must be “point status 3”. Other options lead to errors or unpredictable behavior.

(ii) Best/most predictable results are obtained using “absolute” coordinate systems (see user’s manual chapter 2 section 8 for discussions on coordinate systems)

Step 6. Define individual plates

From the “7-Plate Geometry” screen, select one of either “Circumferential Plates [F2]” or “Longitudinal Plates [F3]”.

Plate segments are defined by pairs of “Near” and “Far” plate points. Each pair has a corresponding edge type. To develop the curved edge to mate with the branch, define and specify a point id (in this case “1”) with a negative sign in front. This technique can be used to create other curvatures, such as a bolt hole.

Do NOT specify non-zero “fillet leg lengths”. This input does not work predictably with generalized structures.

Set “Fine Mesh At” to “none” for linear mesh distribution in the “radial” direction (between point pairs). Do not be too concerned with mesh alignment at this stage. Step 8 must also be completed to ensure that elements will be linearly distributed between near and far points.

Step 7. Apply the individual plate IDs in the “7-Plate Geometry” Screen.

Step 8. Set up Options to improve meshing and Set Stress Calculation Method

Open the “B-Optional” Screen (from the template main menu)

(i) Set the plate mesh tightness to “loose”. This will ensure that the element distributions will be linear.

(ii) Set “Stress averaging” to Gauss-Averaged. This setting will mitigate the geometric singularities in the model.

Step 9. Apply loads to the lug

Open the “2-General” screen (from the template main menu). From the “2-General” screen select “Point Loads [F2]”. Specify the coordinate of the load and the load magnitude as shown below. The load category must also be specified for elastic stress classification rules. (Contact support@paulin.com for help with load categories).

This simplified approach is not intended to provide an accurate calculation for stresses in the proximity of the bolt hole, but gives good results for the lug/base plate junction and elsewhere in the model.

Completed Construction of Model 2

Part 3 - Join the Two Models

At this point the trunnion model (file trun01.ifu) has been setup for database operations and prepared for analysis. We will use the lug model “plate.ifu” as the parent to control the assembly of models.

Step 1. Open the lug model (“plate.ifu”)

Step 2. Open the “2-General” screen from the template main menu. Select “Database operations [F2]”.

Step 3. Set the “Database Read/Write Option” to “2”. This changes the lug model to a “parent” or control model.

Step 4. Specify the child model file name to be connected to the lug model under the “jobnames” column

Step 5. Determine and Input the “Coordinate Shift” of the child model. This action physically locates the child model relative to the lug model.

To determine the “coordinate shift”, it is helpful to find the origin of the two models being combined.

The origin is displayed in a plot of the model using the “advanced” menu. Do this for both models

In this case it is seen that the trunnion model (“trun01.ifu”) only needs to be shifted in the y direction, because the x and z coordinates are on the branch (and lug) centerline. The y direction shift needs to be a distance equal to the height of the branch from the header centerline, or:

ODh/2 + (branch length) = 8.625/2 + 1.38 = 5.6925 inches

Step 6. Plot the combined model to confirm the input coordinate shift is correct.

Step 7. Change the merging method and merging tolerance.

The default database method uses identification numbers, or “join nodes”, to specify how components are assembled. In the “join by proximity” method there are no such identification numbers.

Open the “B-Optional” screen and input the “merge nodes override” (a distance tolerance that should be less than 1/3 the smallest element dimension) and merge nodes method.

The merge nodes method = 0.1 activates the “join by proximity” method. Elements nodes that are within a minimum distance will be considered connected. This minimum distance is specified by the “merge nodes override”. If “0” is specified for a merge nodes override, FE/Pipe will use a value of 0.05 inches (or 0.05 mm if SI units are used). In this example, 0.05 inches is too large for several elements in the trunnion and will lead to “error 3241” during analysis. 0.01 inches was selected by trial and error.

Step 8. Analyze the combined model

Addendum – Overview of Database Operations