Chapter 10: Piping Models

Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index

Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14

10.1 Introduction to Piping Commands

The ANSYS/Multiphysics, ANSYS/Mechanical, ANSYS/Structural, and ANSYS/LinearPlus products offer you a special group of commands that enable you to model piping systems and their loads in terms of conventional piping input data, instead of in terms of standard ANSYS direct-generation modeling operations. As you input piping commands, the program internally converts your piping data to direct-generation model data, and stores the converted information in the database. Once this information is stored, you can list it, display it, modify it, redefine it, etc., using any of the standard direct-generation commands.

10.2 What the Piping Commands Can Do for You

Some special features of the piping module are:

Creates a line model of a piping network using straight pipe (PIPE16) and curved pipe (PIPE18) elements. Node and element geometry is defined in terms of incremental run lengths and bend radii, rather than in terms of absolute coordinates.
Automatically calculates tangency points for bends.
Relates standard piping designations (such as nominal diameter and schedule) to geometric values.
Assigns pipe specifications to element real constants.
Calculates and assigns flexibility and stress intensification factors based on the pressures and the temperatures specified in the pipe module before the creation of the piping elements as appropriate for each element type. The flexibility factors will not be changed automatically if the pipe pressures or temperatures are subsequently revised.
Determines drag pressure loads from a pressure vs. height relationship.

10.3 Modeling Piping Systems with Piping Commands

The procedure for building a model with the piping commands consists of three main steps:

1. Specify the jobname and title.

2. Set up the basic piping data.

3. Define the piping system's geometry.

Further steps required for a piping system analysis include applying additional loads [D, F], etc., obtaining the solution, and reviewing the results. See the ANSYS Basic Analysis Procedures Guide for more information about these other steps.

10.3.1 Specify the Jobname and Title

You perform this step at the Begin level.

First, specify the jobname you want to use for all files that are subsequently created by the analysis [/FILNAME] (Utility Menu>File>Change Jobname).
Next, write an analysis file [/TITLE] (Utility Menu>File>Change Title).
Finally, to write a "reminder" to yourself about the system of units you intend to use, use the /UNITS command. (You cannot access the /UNITS command directly in the GUI.) Remember that /UNITS simply serves as a record for subsequent reviews of the analysis; it does not convert data from one system of units to another.

10.3.2 Set Up the Basic Piping Data

In this step, you take these actions:

To enter PREP7, use one of these methods:

Command(s):

/PREP7

GUI:

Main Menu>Preprocessor

To define the material properties for all materials referenced by the model, use one of these methods:

Command(s):

MPTEMP

GUI:

Main Menu>Preprocessor>Material Props>material option

To select a system of units (if other than consistent), use one of these methods:

Command(s):

PUNIT

GUI:

Main Menu>Preprocessor>Create>Piping Models>Specifications

PUNIT

PDRAG

BRANCH

RUN

BEND

MITER

REDUCE

VALVE

BELLOW

FLANGE

PSPRNG

PGAP

PSPEC

PINSUL

PCORRO

PUNIT

/UNITS

PUNIT

/UNITS

Define the pipe specifications. These specifications will be applied to the elements as they are generated with the RUN command (menu path Main Menu>Preprocessor>Create>Piping Models>Pipe Run).
- To define pipe material and dimensions, use one of these methods:

Command(s):

PSPEC

GUI:

Main Menu>Preprocessor>Create>Piping Models>Specifications

Note-

PSPEC

PFLUID

PINSUL

PCORRO

To define the contained fluid density for a piping run, use the PFLUID command or the equivalent GUI path.
To define the external insulation constants in a piping run, use the PINSUL command or the equivalent GUI path.
To specify the allowable exterior corrosion thickness for a piping run, use the PCORRO command or the equivalent GUI path.

To select the piping analysis standard, use one of these methods: Command(s):

POPT

GUI:

Main Menu>Preprocessor>Create>Piping Models>Specifications

not

Select the pipe loadings.
- To define the pipe wall temperatures in a piping run, use one of these methods:

Command(s):

PTEMP

GUI:

Main Menu>Preprocessor>Create>Piping Models>Loads

Note-

PTEMP

PPRES

PDRAG

To define the internal pressure for a piping run, use the PPRES command or the equivalent GUI path.
To define the external fluid drag loading for a piping run, use the PDRAG command or the equivalent GUI path.

10.3.3 Define the Piping System's Geometry

Define the basic skeleton layout of your piping model.

First, to specify the starting point of your piping system, use one of these methods:

Command(s):

BRANCH

GUI:

Main Menu>Preprocessor>Create>Piping Models>At Node
Main Menu>Preprocessor>Create>Piping Models>At XYZ Loc

Then, follow up with a series of RUN commands (or use the GUI) to define incremental "straight" runs of pipe. (Pipe elements will be generated "straight" in the active coordinate system. See the discussion of "Lines" in Chapter 5 of this guide.) Each RUN command uses length dimensions in the format specified by the PUNIT command to generate a node and a PIPE16 element (along with its real constants, material properties, and loads).

Command(s):

RUN

GUI:

Main Menu>Preprocessor>Create>Piping Models>Pipe Run

Insert bends and other components (tees, valves, reducers, flanges, bellows, and spring restraints) into the model at existing nodes that are shared by two or more existing pipe elements. The program automatically updates your model's geometry to account for the inserted components. Inserted pipe components take their specifications and loadings from the adjacent straight pipes.

To define a bend in a piping run, use one of these methods:

Command(s):

BEND

GUI:

Main Menu>Preprocessor>Create>Piping Models>Elbow

To define a mitered bend in a piping run, use one of these methods:

Command(s):

MITER

GUI:

Main Menu>Preprocessor>Create>Piping Models>Miter

To define a tee in a piping run, use one of these methods:

Command(s):

TEE

GUI:

Main Menu>Preprocessor>Create>Piping Models>Pipe Tee

To define a valve in a piping run, use one of these methods:

Command(s):

VALVE

GUI:

Main Menu>Preprocessor>Create>Piping Models>Valve

To define a reducer in a piping run, use one of these methods:

Command(s):

REDUCE

GUI:

Main Menu>Preprocessor>Create>Piping Models>Reducer

To define a flange in a piping run, use one of these methods:

Command(s):

FLANGE

GUI:

Main Menu>Preprocessor>Create>Piping Models>Flange

To define a bellows in a piping run, use one of these methods:

Command(s):

BELLOW

GUI:

Main Menu>Preprocessor>Create>Piping Models>Bellows

To define a spring constraint in a piping run, use one of these methods:

Command(s):

PSPRNG

GUI:

Main Menu>Preprocessor>Create>Piping Models>Spring Support

To define a spring-gap constraint in a piping run, use one of these methods:

Command(s):

PGAP

GUI:

Main Menu>Preprocessor>Create>Piping Models>Spring-Gap Supp

Another BRANCH command will define the junction point from which another run of pipe branches off of the previously defined run. Subsequent RUN commands will define, in incremental fashion, another run of "straight" pipe elements, starting from the last junction point. The BRANCH and RUN commands and their GUI paths are described earlier in this section.

10.3.3.1 Review and Modify Your Piping Model

Once you have completed your piping data input, you can then review the information that has been stored in the database, using the usual listing and displaying commands [NLIST, NPLOT, ELIST, EPLOT, SFELIST, BFELIST, etc.]. If necessary, you can also modify the data, using standard procedures for revising your model and your loads. (See Chapter 8 of this guide and Chapter 2 of the ANSYS Basic Analysis Procedures Guide for details.)

10.4 Sample Input

Consider the following sample piping data input:

! Sample piping data input
!
/FILNAM,SAMPLE
/TITLE,SAMPLE PIPING INPUT
/UNITS,BIN         ! A reminder that consistent units are British inches
!
/PREP7  
! Define material properties for pipe elements
MP,EX,1,30e6
MP,ALPX,1,8e-6  
MP,DENS,1,.283  
PUNIT,1            ! Units will be read as ft+in+fraction and converted to
                   ! decimal inches
PSPEC,1,8,STD      ! 8-inch standard pipe
POPT,B31.1         ! Piping analysis standard: ANSI B31.1
PTEMP,200          ! Temperature = 200 deg
PPRES,1000         ! Internal pressure = 1000 psi
PDRAG,,,-.2        ! Drag = 0.2 psi in -Z direction at any height (Y)
BRANCH,1,0+12,0+12 ! Start first pipe run at (12",12",0")
RUN,,7+4           ! Run 7'-4" in +Y direction
RUN,9+5+1/2        ! Run 9'-5 1/2" in +X direction
RUN,,,-8+4         ! Run 8'-4" in -Z direction
RUN,,8+4           ! Run 8'-4" in +Y direction
/PNUM,NODE,1
/VIEW,1,1,2,3   
EPLOT              ! Identify node number at which 2nd run starts
BRANCH,4           ! Start second pipe run at node 4
RUN,6+2+1/2        ! Run 6'-2 1/2" in +X direction
TEE,4,WT           ! Insert a tee at node 4
/PNUM,DEFA
/PNUM,ELEM,1
EPLOT              ! Identify element numbers for bend and miter inserts
BEND,1,2,SR        ! Insert a "short-radius" bend between elements 1 and 2
MITER,2,3,LR,2     ! Insert a two-piece miter between elements 2 and 3
/PNUM,DEFA
/PNUM,NODE,1
! Zoom in on miter bend to identify nodes for spring hangers
/ZOOM,  1,  242.93    ,  206.62    , -39.059    ,  26.866    
PSPRNG,14,TRAN,1e4,,0+12     ! Insert Y-direction spring at node 14
PSPRNG,16,TRAN,1e4,,0+12     ! Insert Y-direction spring at node 16
! List and display interpreted input data
/AUTO
/PNUM,DEFA  
EPLOT
NLIST
ELIST
SFELIST
BFELIST

See the descriptions of the PUNIT, PSPEC, POPT, PTEMP, PPRES, PDRAG, BRANCH, TEE, /PNUM, MITER, /ZOOM, PSPRNG, /AUTO, SFELIST, and BFELIST commands in the ANSYS Commands Reference for more information.

Figure 10-1 EPLOT of sample piping input

Go to the beginning of this chapter