Newbanner

 

FE/Pipe with PCL-Gold: Get FEA results without having to learn a new piping or FEA program!

PAULIN Research Group - Frequently Asked Questions (FAQs)
HBar
Table of Contents
(click on a topic listed below to be taken to the FAQ details below)
Installation & Licensing
HBar
FEA Software Installation Error = 931546

This error occurs when attempting to install the software from a CD with a date limit on the installer. You can acquire the full program from the download page on our website. To access the download page, you must setup a membership account. Your account is not tied to your License Number or software registration. Once logged in and on the download page find the file entitled…

 PRG 2007 Release 
Installation program for full release of PRG software. Registration and activation with PRG is required. Note that this installation package is a cumulative installation that includes critical updates and black box fix.

The file above is all of the programs. As a result, it’s about 128 MB. Once downloaded, you may continue the installation as normal. You will need to disable any antivirus software running, as it may prevent a full installation.

 A forewarning though, our program does not work with any odd characters (Such as periods, commas, or slashes. However, Underscores do work) in the path names. Whether it is in the initial install directory or the individual job names. To save your self a hassle and a lot of time please ensure now that it a good install directory.

 C:\PRGSOFT_2007

 Above is an example of a clean directory. (Should be the default) After successfully installing the program, you will still need to authorize it. Please refer to the manual in the installation folder or our installation guides also located on our FAQ page. Should you have any questions about authorization, or any further problems installing, please contact support@paulin.com <back to top>

2551 Fatal Error

 This error generally is a result of running an outdated version of the software. This may happen when installing from a CD. (As opposed to downloading the full release from our website.) The program version is listed under the Help -> About screens on the Main Menu. <back to top>

Technical Errors
HBar

Error ID 3241 and Unzipped Nodes

Error ID 3241

One of the most common errors users have with NozzlePRO is Error ID 3241. There is a simple way of solving this problem by adding a Merge Node Tolerance to the model.

What is error ID 3241?

Every node in the model has an area around it. In order for two nodes to be connected, only two nodes must lie within a certain area. If this area is too large, then three or more nodes may lie within this area collapsing the element. See picture below.

 

FAQ Image1

When does this error occur?

This error occurs most commonly on elliptical heads that have an offset nozzle. The meshing in these cases causes sometimes the collapse of elements due to the complicated meshing that has to be created for these cases.

How do you check for collapsed elements?

There are three important checks the user must look before running a model.

  1. Check for collapsed elements
  2. Check for unzipped nodes
  3. Check for poorly shaped elements

To check for these three important errors, you need to Plot the model. Then in the model window under Controls/Model Verification… you will be able to see the three checks.

FAQ Image2

The second third and fourth of the list are the three most important checks for the model.

If working in FE/Pipe in many cases there can be poorly shaped elements, this can be in the case of Bend with Staunchion, where the meshing on the bend may have poorly shaped elements. These are not as important if they are away from the discontinuity and will not affect the highest stress areas.

Unzipped nodes and collapsed elements are very important. These two must be checked before running any model.

How do we solve error ID 3241?

Adjusting the area mentioned before will solve the error. Usually this error occurs because the area is too large. These can be fixed by changing the Merge Node Tolerance in NozzlePRO and the Merge Node Override in FE/Pipe.

For English units, a good number to start with is 0.005in and for SI units 0.127mm for the Merge Node Tolerance. These are not set in stone though; these values may not solve all of the collapsed elements. The user must keep changing the numbers if collapsed elements can still be seen.

Be careful reducing the Merge Node Tolerance too much, there is a fine line between collapsed elements and unzipped nodes. If the number is too small, then instead of having 2 nodes within a certain area, you will have only 1, meaning that no elements will be connected together. <back to top>

  Unzipped Nodes

When the Merge Node Override is too small, then the elements will not be “glued” together. There is NO error for this. What the user can look for, if this was not checked before running the model, is for unusual high stresses, usually overstressed by more than 300%, when the loadings are small.

As mentioned earlier, the user must be cautious when changing the number in the Merge Node Tolerance box. <back to top>

Why am I getting 2000000000% overstress?

Example: BC.ifu

A common user error in FE/Pipe will give an unrealistic solution such as 2000000000% overstress for any part of the model. The main reason why this could be is due to missing boundary conditions. The other problem that can cause such high magnitudes of stress is due to mismatching midsurface radii in Cylindrical Shells template (STRINGS).

When the user forgets, or does not at a restriction as a boundary condition, then the solution will be very high due to the fact that the model, for FE/Pipe is floating in mid air.

The attached BC.ifu has the problem of boundary conditions. Open this file and run it and you will see in ASME Overstressed Areas under Reports that the stress is 2000000000% overstressed as shown below.

 FAQ Image3

The easy way of fixing this problem is to add a new boundary condition in the Loads/Displacement window as shown below.

FAQ Image4

This boundary condition will tell FE/Pipe that the model is not floating in the air, so results now will be reasonable.

FIXITY is not the only way to add restraints to a model for accurate results. DISPLACEMENT can be added too, the user may fix only certain degrees of freedom, for example, prevent only axial displacement, and leave the rest free to rotate and translate.

FIXITY will fix all 6 degrees of freedom, while DISPLACEMENT will have to specified by the user which degrees of freedom to keep fixed.

There are some other cases that can have this same problem, but it is not due to boundary conditions. In the Cylindrical Strings Template (STRINGS), this problem might occur if there is an input error in the midsurface radius specified by the user. This usually happens when a skirt is being added, and the midsurface radius of the skirt does not match the midsurface radius of the vessel shell. The user should careful check all the midsurface radii when getting these unrealistic results. <back to top>

 

General
HBar
Nozzle and Header/Pad Definitions - Regions

Regions are defined differently in different FE/Pipe Templates. Below are the definitions for 4 common templates:

Nozzle and Pad Definitions (General Nozzles, Shells and Plates)

 Nozzles are divided into 3 sections:

  1. Nozzle at Junction
  2. Nozzle Transition
  3. Nozzle Away from Junction

The pad is divided in 3 sections:

  1. Nozzle # at weld pad area
  2. Pad next to Nozzle #
  3. Pad at nozzle #

The discontinuity in the shell is divided in two sections:

  1. Shell at Nozzle #
  2. Shell in Nozzle # Vicinity

The meshing and dimensions of these three parts of the nozzle can be adjusted by the user. Please see Hillside Nozzle.

FAQ Image5 <back to top>


Nozzle and Pad Definitions (Reinforced Fabricated Tee)

 Branches are divided into 3 sections:

  1. Branch at Junction
  2. Branch Transition
  3. Branch Removed from Junction

The Header/Pad is divided in 3 sections:

  1. Header/Pad at Junction
  2. Pad Removed from Junction
  3. Pad Outer Edge Weld

The Header has one section:

  1. Header outside Pad Area

 FAQ Image6 <back to top>

 Nozzle and Pad Definitions (Unreinforced Fabricated Tee)

 Branches are divided into 3 sections:

  1. Branch Next to Header Weld
  2. Branch Transition
  3. Branch Away from Junction

The Header is divided in 3 sections:

  1. Header Next to Nozzle Weld
  2. Header Away from Junction

FAQ Image7 <back to top>

Branch and Run Definitions (Welding Tee)

Branches are divided into 2 sections:

  1. Transition to Top Pipe
  2. Top Pipe

Run/Header is divided into 4 sections:

  1. Transition to Front Pipe
  2. Front Pipe
  3. Transition to Back Pipe
  4. Back Pipe

Tee is divided into 2 sections:

  1. Tee Body
  2. Crotch Area

ImgWeldTee<back to top>

What are the definitions of FE/Pipe’s boundary conditions?

 There are many types of boundary conditions in FE/Pipe. Below is a list of all boundary conditions.

  • FIXITY
  • DISPLACEMENT
  • FORCE
  • HEAD
  • RIGID
  • FLAT
  • PFIX
  • SYMFIX
  • NONE

FIXITY – Fixity will restrain all 6 degrees of freedom, not translation or rotation will be allowed at the specified node selected by the user. There is some radial displacement allowed in this boundary condition. If the user does not want any radial displacement, then RIGID should be used, see definition below.

DISPLACEMENT – The user can specify which displacements are allowed. The figure below shows the only allowed displacement in the FY direction and rotation in the RX axis.

FAQ Image8

“Free” can be placed by the user saying that this degree of freedom is free to translate or rotate. Note that the Weight and Operating case were both entered with the same values, these two are different cases and will be computed as separate load cases, and therefore it is a good idea to place the same values on both, if the user does not have different values for Weight.

FORCE – The user can add forces in any direction.

HEAD – For vessels, sometimes the user needs to model the top of the vessel to have a head boundary condition. FE/Pipe will add a head to the model so that the top of the vessel is not free to rotate or displace in any direction. The type of head placed is defined in the Optional window (only for NOZSHELL template).

RIGID – This boundary condition will place a rigid element at the desired location, this boundary condition will add stiffness, that is prevent radial displacement also, to the model as well as restrict it from moving in all 6 degrees of freedom.

FLAT – This boundary condition is very much alike HEAD boundary condition, only this time a flat plate will be added to the top of the vessel or nozzle, to prevent some radial displacement and some rotation.

PFIX – This will allow displacement in the axial direction. Usually what is used for a vessel is FIXITY at the bottom and PFIX at the top. PFIX allows axial displacement so that accurate PD/4t stresses can be computed at the boundary condition due to pressure.

SYMFIX – Provides axial restraint and local in-plane bending restraint. This boundary condition is more commonly used when only half of a symmetric model is used.

NONE – No boundary condition will be applied. <back to top>

Why is there a missing band of material in the plotted results on output graphics as shown below?

 FAQ Image9

The non-rendered region is the zone within one-half the wall thickness of the pressure vessel head or one-half the wall thickness of the nozzle plus fillet weld lengths.  In the case of very thick head, shell or nozzle, the region is rather wide.

 This approach (not using stresses within the volume of the intersection) has been supported by past Pressure Vessel Research Council (PVRC) publications and is also supported by the new ASME Section VIII, Division 2, Annex 5.A.  The concept is that the stresses within the intersection volume do not represent valid membrane or bending stresses.  However, the stresses in the shells directly adjacent to this zone are valid.  Therefore, our reports begin at the edge of the intersection plus any fillet weld that is specified.

 This procedure is good practice regardless of the type of finite element tool being used.  For instance, if you are using a product like ANSYS®, you should be reporting stresses at a similar region.  Stresses within the volume of the weld have no physical meaning and should be discarded.  This is often not done because: 1) analysts do not understand the intent of the Code, 2) it is too difficult and time consuming to do with general FEA tools. <back to top>

What are the definitions for Inplane, Outplane, Torsional and Axial for Intersections and Bends?

Inplane, Outplane, Axial and Torsional Directions

  • Inplane Force/Moment: Is a force or moment that will cause the branch to deflect towards the header along its centerline.
  • Outplane Force/Moment: Is a force or moment that will cause the branch to deflect along the circumferential plane of the header.
  • Torsional Force/Moment: Is a force or moment that will cause the branch to deflect around its centerline.
  • Axial Force: Is a force that will cause the branch to deflect along its centerline.

All inplane, outplane, torsional and axial directions are in the local axis. For laterals the same process will be applied regardless of the angle of tilt of the branch to header. <back to top>

 For Intersections (Tees and Heads):

 FAQ Image10

For a center nozzle on a head, the inplane and outplane direction will be the same. <back to top>

For Bends and Bends with Support:

FAQ Image11 <back to top>