Paulin Research Group                   Houston, Texas

 

Hillside Nozzle Meshing Adjustment in General Nozzles, Plates and Shells

Example Model: hillsid2.ifu

 

Nozzles in FE/Pipe are broken down into three sections: Nozzle at Junction, Nozzle Transitions and Nozzle Away from Junction. Please see: What is Nozzle Next to Junction or Nozzle Transition? 

When the user enters an offset for a nozzle, the default meshing for many cases is not going to give a decent model. The main reason why is because the Nozzle at Junction part of the nozzle is too small for the proper meshing. This section needs to be larger than the distance taken from the nozzle by the curvature of the shell.

 

In this example we are going to properly mesh a hillside nozzle.

 

  1. Open FE/Pipe and create a new file.

 

 

2.      Select General Nozzles, Plates and Shells.

 

3.      Select Shell Geometry and enter the outer diameter of the vessel, the thickness and the length. We are going to add an elliptical head with an ellipse ratio of 2.

 

4.      Select Nozzle Geometry. Here is where the hillside is defined. The Optional Nozzle Orientation Vector is the one that defined the hillside. The nozzles will always be at the surface, but defining the Optional Nozzle Orientation Vector to be in the –Z direction, will make the nozzle be hillside.

 

 

We can see in the Optional Nozzle data that the Reinforced Nozzle Length is set to 25in, the Nozzle Length to 5in and the Transition Length to 2in. The Nozzle Reinforced Length will be the part of the nozzle that is closer to the junction (i.e. Nozzle at Junction), and this part needs to be larger than the curvature created by the shell as shown in the picture below.

 

The user needs to keep increasing this number until there is a proper mesh. If this number is too small, then the meshing will have unattached parts that will be easy to see when plotting the model.

 

The nozzle in this case will be 32 inches long, 25in + 2in + 5in = 32in.

 

  1. After the nozzle is defined, we can plot the model and see the hillside nozzle. Next, what needs to be done is to add boundary conditions and loads as well as the meshing parameters. Select Shell Boundary Conditions. For the bottom the closer to reality is FIXITY. No movement will be allowed in any of the 6 degrees of freedom. For the top, HEAD is the one that we are looking for, so that a head will be placed at the top of the model.

 

  1. Select Nozzle Miscellaneous. In this window we can control the meshing of the nozzle.

 

Notice that the Nozzle Number has to match the number placed in Nozzle Geometry. In this case we are going to select to compute SIF’s and Flexibilities for this nozzle.

 

The Stress Concentration Factors are used to find Peak Stresses for fatigue analysis. The default value is 1.35, these numbers can be changed by the user, but 1.35 seems to be a number that agrees with experimental data from PRG and from past experience.

 

Removing plug from the header can be switched from YES to NO if a lifting trunnion is to be analyzed. The difference in stresses can be significant from switching from NO to YES and vice-versa.

 

If only the hole wants to be analyzed and not the nozzle, then the user can select to remove the nozzle and leave the hole for analysis by changing “Remove or Taper Nozzle” from NO to YES.

 

Insert Nozzles are also specified in this window, the length of the insert nozzle cam be specified in “Insert Nozzle Penetration Length”.

 

The meshing parameters are at the bottom of the window.

 

The “Elements in Nozzle at Junction” is defined as 12, as this is the longest part of the nozzle in this case. We set this to be 25in long. The default was left as it is for “Transition” and for “Nozzle Away from Junction”.

 

The reinforcing pad can be meshed too, and this is set in this window too under “Elements in Reinforcing Pad”.

 

  1. After the meshing is done, the material properties need to be entered. Select Shell Properties.

 

Enter the material properties of the shell and head. We entered the allowable stresses for carbon steel. A 0.01psi was entered in order to enable the software to compute SIF’s and Flexibilities. In FE/Pipe and NozzlePRO, a pressure needs to be added for proper computation of SIF’s, even if no loads are defined.

 

  1. Select Nozzle/Plate Properties.

 

We entered the Nozzle number and then the allowable stresses for carbon steel. Notice that only the hot and cold allowable stresses are required, not the Tensile Strength or hot or cold yield stresses.

 

  1. The model is ready to be plotted and verified. Press F-Prepare for Analysis. Then go to Controls/Model Verification…

 

  1.  Select Show collapsed elements and press ok. The model should disappear, leaving a blank screen. This means that there are no collapsed elements. If you see blue lines, this means that you have collapsed elements and the Merge Node Override needs to be adjusted (See How can I fix Error ID 3241 or Unzipped Nodes? in Frequently Asked Questions).

 

  1.  Go to controls and Model Verification again and select “Show Unzipped nodes in model”. Only black circles should be shown at the bottom of the shell.

 

 

If unzipped nodes are found anywhere else, please correct the Merge Node Override (See How can I fix Error ID 3241 or Unzipped Nodes? In Frequently Asked Questions)

 

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

 

 

Nozzle SIF can be seen here, and there is a comparison between the FEA SIF’s with the B31.2, B31.1 and WRC 330 SIF’s.

 

The Flexibilities:

 

The allowable loads:

 

 

 

Back to Top