• Pipe Parts:

• All Types of Fittings

• Elbow Parts
• Flanges
• Reducers
• Other Fittings

SolidWorks Piping-"isms"

When creating SolidWorks Parts to be used in the context of a SolidWorks Piping Assembly (using the SolidWorks Piping Add-on) there are some things to consider:

This is a summary of the features, sketches, and dimensions that you must use in the components of piping assemblies. For more detailed information, see the topics for each component type. NOTE: The software identifies parts as potential piping components when it detects the presence of certain items. Some properties are added automatically to such parts. These properties, named Component type and Fabricated pipe parts, are listed on the Custom tab of the Summary Info dialog box (click File, Properties). They are not configuration-specific. Do not delete these properties or edit the values that are assigned to them. See also Connection Point and Route Point .

• A sketch named PipeSketch, consisting of two concentric circles with dimensions named OuterDiameter and InnerDiameter
• An extruded base feature, named Extrusion,with a depth dimension named Length.
• A sketch named FilterSketch, consisting of a circle with a dimension named NominalDiameter.
• A configuration-specific property named $PRP@Pipe Identifier (value must be unique for each configuration).
• A configuration-specific property named $PRP@Specification (recommended).
• A design table with a configuration for each size of raw stock that you use.

1. InnerDiameter@PipeSketch
2. OuterDiameter@PipeSketch
3. NominalDiameter@FilterSketch
4. $PRP@Pipe Identifier
5. $PRP@Specification
6. Note: Do not include Length@Extrusion in the design table.

In any fitting part that has multiple configurations, Specification@Cpointn is recommended for each connection point (include as a design table parameter).

• A sketch named ElbowArc, consisting of an arc with dimensions named BendAngle and BendRadius.
• A sweep feature for the base, using ElbowArc as the sweep path.
• The sweep profile is a sketch that contains one circle.
• A Connection Point at each end of the elbow, where you want the pipe to be cut.
• A design table with a configuration for each size of elbow that you use.
• You must include the following parameters in the table:

• BendAngle@ElbowArc
• BendRadius@ElbowArc
• Diameter@Cpointn (for each connection point)

• One Connection Point
• A design table with a configuration for each size of elbow that you use.
• You must include the following parameter in the table:

Diameter@Cpointn (for each connection point)


A Mate Reference is required in each flange to allow the component to "snap" to the tank or pump to begin the spool. NOTE: Currently (with SolidWorks 2001+) only one mate reference is allowed per part. It has been found that moving (or mating) the spool after it has been been placed in the Assembly has caused corruption to the assembly model(s) and should be avoided.

• One Connection Point at each end

• One Connection Point at each port
• One Route Point at the intersection of the branches

This document maintained by Jeffrey P. Kuchta.
Material Copyright © 2002 {Jeffrey P. Kuchta}