Building a model with the piping commands consists of three primary tasks:
All piping commands referenced here are described in Part II: Archived Commands.
Other actions required for a piping system analysis include applying additional loads (D, F, etc.), obtaining the solution, and reviewing the results. See the Basic Analysis Guide for more information.
Perform these steps at the Begin level.
Set up the basic piping data as follows:
Enter PREP7 (/PREP7).
Define the material properties for all materials referenced by the model (MP, MPTEMP, etc.).
Select a system of units, if other than consistent (PUNIT).
The PUNIT command determines how the program interprets the data input for the PDRAG, BRANCH, RUN, BEND, MITER, REDUCE, VALVE, BELLOW, FLANGE, PSPRNG, PGAP, /PSPEC, PINSUL, and PCORRO commands. The difference between PUNIT and the /UNITS command is that PUNIT affects how the program behaves, whereas /UNITS does not.
Define the pipe specifications. These specifications are applied to the elements as they are generated via the RUN command.
Define pipe material and dimensions (PSPEC).
Define the contained fluid density for a piping run (PFLUID).
Define the external insulation constants in a piping run (PINSUL).
Specify the allowable exterior corrosion thickness for a piping run (PCORRO).
Select the piping analysis standard (POPT).:
The program calculates and assigns flexibility and stress intensification factors for curved pipe elements 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 and stress intensification factors are not changed retroactively if the pipe pressures or temperatures are subsequently revised.
Select the pipe loadings.
Define the pipe wall temperatures in a piping run (PTEMP).
Define the internal pressure for a piping run (PPRES).
Define the external fluid drag loading for a piping run (PDRAG).
Define the basic skeleton layout of your piping model as follows.
Specify the starting point of your piping system (BRANCH).
Follow up with a series of RUN commands to define incremental "straight" runs of pipe.
Pipe elements are generated "straight" in the active coordinate system. 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).
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, issue the BEND command.
To define a mitered bend in a piping run, issue the MITER command.
To define a tee in a piping run, issue the TEE command.
To define a valve in a piping run, issue the VALVE command.
To define a reducer in a piping run, issue the REDUCE command.
To define a flange in a piping run, issue the FLANGE command.
To define a bellows in a piping run, issue the BELLOW command.
To define a spring constraint in a piping run, issue the PSPRNG command.
To define a spring-gap constraint in a piping run, issue the PGAP command.
Another BRANCH command defines the junction point from which another run of pipe branches off the previously defined run. Subsequent RUN commands define, in incremental fashion, another run of "straight" pipe elements, starting from the last junction point.
When you have completed piping data input, you can review the information that has been stored in the database via standard listing and display commands (NLIST, NPLOT, ELIST, EPLOT, SFELIST, BFELIST, etc.).
If necessary, you can modify the data using standard procedures for revising your model and your loads. See Loading in the Basic Analysis Guide for details.