Solid Edge Solid Edge Standard Parts – Creating Custom Pipes

2021-10-06T23:58:53Z

APPLICATION

Summary

Details

The goal is to add a custom pipe component to the Solid Edge Standard Parts library that can be used with the XpresRoute – Piping Route utility.

Solution

Preparation:

1. First create a base profile you will use to build your custom pipe category. The base feature is Ordered and always an Extrude (not a revolved extrude!). Save it with a name that will help you recognize the pipe e.g. Dairy Pipe_BS4825_127x16.par.

2. Start the PreparePipingComponents.exe macro to prepare your pipe.

3. Use the Prepare Pipe option and define the input and output diameter and select the two pipe openings. This utility will add the coordinate systems required for the library and will add a variable "LL" and "Diameter_1" to control the dimensions.

Add component to Standard parts

Next step is to add this custom component to the Solid Edge Standard parts Library.

1. Start the Standard parts Administrator.
2. Add Parts -> Add new user part file(s).
3. Add from manual data entry.
4. Select the part.

5. Select Piping part; a pipe has 2 CS pairs.

6. Create a new category for your custom parts.

7. Add Characteristics.

This is the most critical step for the Piping Route utility. Selection of the available pipes is related to the characteristics "Nominal pipe size" and "Outside diameter".

Note:

There are two types of characteristics - constant and variable. For a variable characteristic (e.g. for pipes and structural shapes length) a variable must be set in the appropriate cell of the Properties grid and this variable should correspond to a variable existing in the source parts. Conversely, a more common constant characteristic must not have set any variable in the Variable column. For every characteristic a unit class and appropriate unit must be set.

8. Enter the coordinate system's parameters according to the appendix in the Standard Parts help section.

In this example:

INPUT_POINT_1.CD = 10 (Connecting diameter of the opening)
INPUT_POINT_1.ET = 0 (End Treatment)
INPUT_POINT_1.IO = 1 (Type of CS)
INPUT_POINT_1.NS = 12,7 (Nominal Size)
INPUT_POINT_1.SN = 1 (Sequence number)
INPUT_POINT_1.WT = 1,6 (Wall Thickness)

OUTPUT_POINT_1.CD = 10 (Connecting diameter of the opening)
OUTPUT_POINT_1.ET = 0 (End Treatment)
OUTPUT_POINT_1.IO = 2 (Type of CS)
OUTPUT_POINT_1.NS = 12,7 (Nominal Size)
OUTPUT_POINT_1.SN = 1 (Sequence number)
OUTPUT_POINT_1.WT = 1,6 (Wall Thickness)

INPUT_POINT_2.CD = 10 (Connecting diameter of the opening)
INPUT_POINT_2.ET = 0 (End Treatment)
INPUT_POINT_2.IO = 1 (Type of CS)
INPUT_POINT_2.NS = 12,7 (Nominal Size)
INPUT_POINT_2.SN = 2 (Sequence number)
INPUT_POINT_2.WT = 1,6 (Wall Thickness)

OUTPUT_POINT_2.CD = 10 (Connecting diameter of the opening)
OUTPUT_POINT_2.ET = 0 (End Treatment)
OUTPUT_POINT_2.IO = 1 (Type of CS)
OUTPUT_POINT_2.NS = 12,7 (Nominal Size)
OUTPUT_POINT_2.SN = 2 (Sequence number)
OUTPUT_POINT_2.WT = 1,6 (Wall Thickness)

9. Select a visual navigation category.

10. Part will be generated.

You can repeat these steps for all additional sizes you need in this category. You need to create a master part for every diameter/wall thickness needed.

Test result

1. Create a new assembly.
2. Open the Standard parts Library.