Wes Mosler - The Piping and Tubing Design Guide for SolidWorks Routing

the piping and tubing design guide for solidworks routing là bộ tài liệu hướng dẫn đầy đủ nhất về phần đường ống và hệ thống đường ống, tính toán mô phỏng trên phần mềm solidworks. Tài liệu hướng dẫn chi tiết, dễ thực hành, nó đủ hữu dụng cho người mới bắt đầu tới nâng cao.

The Piping & Tubing

Design Guide

for SolidWorks Routing 2011

By: Wes Mosier

This Page Intentionally Left Blank

SolidWorks Routing 2011

Piping & Tubing Design Guide

This manual is meant for instructional use only, and is in no way intended to replace the SolidWorks Routing help files or the SolidWorks Manual

In case of conflict, always refer to the documentation

supplied with your SolidWorks license

SolidWorks is a registered trademark of

SolidWorks Corporation

SolidWorks Corporation is a Dassault Systemes S.A company

SolidWorks Corporation

300 Baker Avenue Concord, Massachusetts 01742 USA

This reference manual was prepared by:

Wes Mosier

Copyright © 2004, 2005, 2006, 2007, 2008, 2009, 2010 & 2011 - Wes Mosier

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Typical piping skid

Image Courtesy of Wes Mosier

Table of Contents

Chapter 1 – The Basics

How the Routing Package Works……… 1-1

Cpoints & Rpoints……… 1-1 Design Tables……… 1-2 The 3D Sketch……… 1-4 Assemblies, Subassemblies, Parts & Routing Files……… … 1-6 Routing Templates……… 1-8 How They All Work Together……… 1-9 Routing Options and Settings……… 1-11

Chapter 2 - Required Features of Components

Cpoints & Rpoints (What are they?)……… 2-1 Pipe……… … 2-5 Tube……… 2-8 Elbows……… ……… 2-12 Tees……….……… 2-16 Flanges……….……… 2-17 Reducers……….……… 2-17 Other Components (Valves, Filters, Strainers, etc…)……….………… 2-18

Chapter 3 – Starting a Route (creating a routing subassembly)

Things to consider before starting……… 3-1 The Design Library……… 3-2 Adding a starting component to the assembly……… 3-4 The Route Properties Dialog……… 3-5

Chapter 4 – Routing Pipe

Route Properties/Settings……… 4-1 Routing Straight Pipe With Elbows……… 4-3 Routing Bent Pipe……… 4-7 Ending Your Route……… 4-10 Creating Custom Elbows (when you exit the sketch)……… 4-11 Piping Routing Files……… 4-14

Chapter 5 – Routing Tubing

Route Properties/Settings……… 5-1 Routing Rigid Tube……… 5-3 Routing Flexible Tubing 5-4 Ending Your Route………5-6 Tubing Routing Files……… 5-7

Chapter 6 – Editing a Routing Subassembly

Adding a Tee……… 6-1 Adding Components to Your Route……… 6-6 Using Split Points to Add Components to Your Route……… 6-11 Removing Pipe or Tube Between Two Fittings……… 6-13 Adding Back Removed Pipe or Tube……… 6-15 Adding a Reducer to Your Piping Route……… 6-16 Changing the Route Properties……… 6-24 Changing the Line Size/Schedule of Your Pipe/Tubing Route….………… 6-26 Replacing Routing Components ……… 6-29

Chapter 7 – Miscellaneous Routing Procedures

Pipe Penetrations……… 7-1 Adding Mounting Brackets & Pipe Supports……… 7-3 Forming Subassemblies……… 7-10 Dissolving Subassemblies……… … 7-10 Using “Find References” to Relocate Pipe/Tubing Files………… ………… 7-11 Bolted Connections……….……… 7-12 Adding Branch Fittings (Weld-O-Lets & Bosses)……… 7-13

Chapter 8 – Creating Custom Routing Components

Creating Custom Components (Valves, Strainers, etc…)……… 8-1

Cpoints………… ………8-2 Rpoints……… 8-4 The Vertical Axis……… 8-6 Creating Custom Flanges & Start Parts……… 8-7

Chapter 9 – Inserting Subassemblies Into Your Route

Creating a Routing Subassembly……… 9-2 ACpoints & ARpoints……… 9-4 Inserting the Subassembly Into Your Route……… 9-6

Chapter 10 – Design Tables

What Exactly Does the Design Table Do?……… ……… 10-1 Adding Custom Properties………10-2 Pulling the Data Out of the Design Table & Into My Drawing……….10-4

Chapter 11 – The Drawing

How to Crop Pipe So It Looks Like Pipe……… 11-1 Dimensioning Pipe & Tubing……… 11-2 The Bill of Materials……… 11-3

About This Manual:

The information provided in this manual is meant as a supplement to the online help files and documentation provided with your copy of SolidWorks 2008 and the

SolidWorks 2008 Routing add-on In case of conflicting/missing information, always consult the documentation and help files supplied with your copy of SolidWorks

About the Author: Wes Mosier, CSWA, CSWP, CSWE

Wes Mosier has been involved in the mechanical design, architecture, structural and process piping industries for over nineteen years as a Cad Engineering Design Drafter

He has written procedural manuals and technical documentation for large and small companies over the past 12 years, and has taught both lecture and hands on courses at private firms and technical conventions, including break-out classes at

SolidWorks World

Wes Mosier has been using the SolidWorks Piping/Routing add-on for over 10 years while employed by engineering, fabrication and design firms in California

“I wrote this manual to give the users of SolidWorks Routing a heads-up

approach to learning the basics of the tubing and piping package Individuals who follow this document can gain a clear understanding of the fundamentals behind how the program works, and can adapt these procedures to suit their specific company needs Simply put, this manual was written by a user, for the user.”

-Wes Mosier

Special thanks to my wife Kelly, for putting up with my late nights and for all the encouragement

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Chapter 1 – The Basics

Step One: Turn on SolidWorks Routed Systems

Is SolidWorks Routing Included in my Version of SolidWorks?

SolidWorks Routed Systems comes included with SolidWorks Premium It is not a part of the SolidWorks Professional package It is easy to upgrade from Pro to Premium Simply contact your reseller, and they will provide you with all of the necessary

information They can also tell you about all of the additional benefits and features available with the Premium package

To see which type of SolidWorks you currently have installed, open SolidWorks, and click

“Help” on the top menu bar, then “About” towards the bottom of the drop-down

Your type of

SolidWorks will

be shown here

A quick note about the name:

Throughout this manual, I will refer to SolidWorks Routing as both SolidWorks Routed Systems

& SolidWorks Routing In the early days of the software, it was originally called SolidWorks Piping, then changed to SolidWorks Routing when the electrical enhancements were added The current “official” name is “SolidWorks Routed Systems”, but is widely known by any of these names Depending on what country you are in, the spelling may be slightly different, but it is all

the same software

Activate the Routed Systems Add-In

When you are positive that you have SolidWorks Premium edition, you must then be sure the Add-In for Routed Systems is enabled To do this, simply select “Tools” from the top menu bar, then select “Add-Ins” towards the bottom A window will appear displaying all

of the add-ins that you have installed Scroll down the list, and find the one called

“SolidWorks Routing”

If you do not see “SolidWorks Routing” in the list, then you either do not have

“SolidWorks Premium” edition, or for some reason, the Routing Add-In was not installed when you originally installed SolidWorks Contact your reseller for more information on either of these two cases

By checking the box to the left of the “SolidWorks Routing” name, you will activate the add-in for this current session of SolidWorks only If you check the box to the right of the name, Routing will activate every time you start SolidWorks

It is recommended that you disable the add-in when not in use to conserve memory and other computer resources

Click the “OK” button and SolidWorks will load Routed Systems into memory This will include adding approximately (5) five floating toolbars and a “Routing” drop-down to the top menu bar You will not need all of these toolbars to route piping and tubing Some

of the toolbars contain electrical routing tools, and some of the toolbars are simply

smaller versions of the larger ones

How the Routing Package Works

At first glance, SolidWorks Routing would seem to be a very complex, hard to understand add-in Although it is considered an advanced topic, it is actually quite simplistic in its design and utilizes basic SolidWorks principles to complete the routing tasks Having a solid understanding of how SolidWorks functions, top-down design, creating parts, and editing assemblies in context is a prerequisite to learning SolidWorks Routing

When you create a route in SolidWorks, you are really just creating an in-context subassembly and creating a 3D Sketch to tell SolidWorks where your route goes You can add components to your route by dragging and dropping them onto sketch points

You have probably already used most of the tools that SolidWorks Routing utilizes to create parts and assemblies Some of these are Design Tables, 3D sketches, working In-Context, Parts and Subassemblies Some other tools may be new to you like Cpoints and Rpoints

Cpoints & Rpoints

Every component that is used in a piping or tubing route must have some sort of identifier that tells SolidWorks that it can be used with the Routing package That is what Cpoints

& Rpoints do

Cpoints tell SolidWorks where to start a piece of pipe or tube from (such as the end of

an elbow where a piece of pipe would be buttwelded) They also contain routing

properties that tell SolidWorks what size of pipe/tubing to route, and what direction it goes (away from the fitting, or towards it) There are three types of Cpoints: Fabricated Pipe, Tubing and Electrical The type you use depends on what you want to route Some parts contain both Tube Cpoints and Fabricated Pipe Cpoints, such as a pipe to tube adapter The image below shows a typical buttwelded TEE pipe fitting Notice that the Rpoint is on the intersecting points of the part, and the Cpoints are on the ends When sketching your route, the Rpoint would be placed onto the point at the intersection of the segments

Rpoints are used to locate the component on a point in the 3D Sketch, hence the name

Route Point or Rpoint When placing a component into a piping route, the Rpoints of components can be placed at the end point of a line, or on a “Split Point” in the 3D sketch

Cpoint

Rpoint Cpoint

Cpoint

There are also variations of the Cpoints and Rpoints that are used in subassembly components These are called ACpoints & ARpoints These are used when inserting a subassembly into a route I'll show you how to do that in Chapter 9, "Inserting

Subassemblies Into Your Route"

See also:

Chapter 2 – Cpoints & Rpoints

Chapter 9 – ACpoints & ARpoints

Design Tables

Think of a design table as nothing more than a spread-sheet style representation of all the variables in configurations Design Tables have commonly been used in SolidWorks

parts and assemblies to show different variations of a part or assembly (See the

SolidWorks help files for more information on creating and editing Design Tables for standard parts and assemblies, and Chapter 10, Creating Design Tables)

The cylinder shown here has two configurations in the

part file One configuration says that the diameter is

2” and is extruded 1” The other has a diameter of 1”

The design table for the standard library pipe file looks something like this:

Column “A” contains all of the configuration names

Column “B” has the part number for that configuration

Column “C” contains the pipe identifier (remember this column data for later)

Column “D” shows the nominal diameter of the pipe

Column “E” is the actual O.D of the pipe

Column “F” lists the wall thickness of the pipe

Column “G” is a calculated I.D of the pipe

Column “H” shows the weight per foot of pipe

Most of these columns are linked directly to sketches used in the part, while others are linked to feature dimensions or properties Any column that has a “$prp@” in front of it is linked to a custom property in your part or assembly

SolidWorks uses this information to display the pipe on the screen in the 3D sketch, creates a routing file when you exit the 3D sketch after routing a pipe, and to display this information in the drawing’s bill of materials

Other columns can be added to the Design Table including Material, Chamfer

information, Specifications, Manufacturing Notes, Purchasing Information, special notes

on each type of pipe, and even color

Elbow files, Tees, and many other piping/tubing components all use design tables to allow the user to quickly organize, display, add to, and alter the raw data that SolidWorks uses to create your route A custom valve without any configurations would not need a design table to be used in a route

See also:

Chapter 10 – Design Tables, Adding Custom Properties

The 3D Sketch

In SolidWorks, you need a way to draw the path of your pipe or tubing You do this using

a 3D sketch This allows you to run a layout in any direction, using any dimensions or constraints that you would normally use in a 3D sketch

3D Sketches are commonly used in parts to draw a path that can be used as a sweep

extrusion path When you draw a route in the 3D sketch, SolidWorks basically extrudes

the pipe or tube along that same path

When you start a new route, SolidWorks automatically opens a new 3D sketch for you to draw with inside of a new subassembly

While routing in a 3D Sketch After Exiting the 3D Sketch

As you draw your routing lines, SolidWorks displays a piece of pipe at the nominal size that is taken from the pipe or tube design table You can tell the routing package to add bends automatically, and if you so choose, elbows can be placed automatically on the bends when you exit the 3D sketch

You can use Sketch Planes, Sketch Relations, Construction Lines, and Dimensions to further define your Routing Sketch, just like you would with any other 3D Sketch you make It is recommended that you fully define your route sketch, or things might mysteriously move without warning.

See also:

Chapter 1 – Routing Options & Settings

Chapter 3 – Starting a Route

Chapter 4 – Routing Pipe

Chapter 5 – Routing Tubing

Assemblies, Subassemblies, Parts & Routing Files

An assembly is just a file that contains multiple parts and subassemblies

A subassembly is nothing more than an assembly that is inside of another assembly (basically, a nested assembly) It too can contain more subassemblies and parts When you're using the Routing Package, the subassembly also contains the 3D Sketch that is used to create your route

Parts are components such as elbows, valves, flanges, etc… that are brought into a routing subassembly to form a “route”

Routing files are part files that SW will create from the Pipe and Tube “Base part files” when you exit a 3D sketch I'll explain the “Base part files” more a bit later in this chapter These files can either be saved externally like a normal part or virtually inside the routing subassembly

Let's just say that I create a new assembly and start a route (the route automatically turns into a subassembly) and bring parts into my route like flanges and tees I now have the main (top level) assembly that I started with and a routing

subassembly inside it that contains all the routing components (parts) and routing files (more parts that are the individual pipe segments)

This might sound a little confusing at first, but maybe it will help if I give you a real world example:

Let’s say I open a new assembly and save it, (I cannot start a route in a new assembly that has never been saved) and then insert a 4” flange from the Design Library, and start a new route

The new route will be the routing subassembly inside my main (top level) assembly I can have multiple routing subassemblies in my main assembly to form complete piping and tubing systems

In my route, I use 4” schedule 40 pipe, and drew some sketch lines up, then over, then down When I exit the 3D sketch, SolidWorks will automatically create a

“virtual subassembly” inside this top level assembly that contains a “virtual” pipe part that

is a modified version of the Pipe Identifier Property of the pipe file I selected when I started the route That “virtual” pipe part will contain configurations for all the different lengths of pipe I just created (The Pipe Identifier is taken from the design table of the

base pipe part file that I selected when I started the route, and is slightly modified to remove any commas or special characters.)

When I save my top level assembly, SolidWorks will tell me that my assembly contains some “virtual components” and ask if I want to save them out to a separate file,

or keep them virtual inside the assembly

See Chapter 4 – Piping Route Files

The above example is based on routing fabricated pipe with elbows, and will vary slightly if you are routing bent pipe, or tubing You may also have set your Routing Options differently to automatically save out the parts instead of creating virtual

automatically assigned based on a derivative of the pipe identifier property (see page 3) used in the Base Pipe Part file that was selected when you started the route The “^” also tells you it is a Virtual Part inside of the TransferLine subassembly

1-Next to every Route Part, the instance count is shown between the <>, and the

configuration name is shown in parenthesis In the above condition, the Route Parts are stored as Virtual Components inside the TransferLine.sldasm subassembly

A typical “routing file” would look like this in the Feature Tree:

06-STD-A106B <3> (06-STD-A106B,3) 11.43in

Part File Name

3rd time this file is used in this subassembly

This is the name of the configuration being used

This is the length of the piece of pipe in the route

Routing Templates

Templates are used throughout SolidWorks as a base file for creating new parts,

assemblies and routes For example, if you were to open SolidWorks and start a new part, SolidWorks will open the Part.prtdot template file, and use it for your new part The template file contains all of the information pertinent to starting a new file, such as units, colors, settings, grid size, options, document properties, etc…

Routing templates are no different You can customize how your Routing

Subassemblies begin by editing the routing template For example, you can add extra planes in the template to specify elevations, set up project specific units, or you can create a base-sketch of the floorplan of a building and use it as a reference to route your piping that includes grid lines, coordinates, etc

It is recommended that you edit an existing routing template file, then save it as your own custom template, rather than start a new assembly and save it in the template format

Every time you start a new route, you can specify the routing template for that project, and have all of your routing subassemblies use the same template

The default template file is located in the

“SolidWorks\Data\Templates” directory and is

called “routeAssembly.asmdot”

How They All Work Together

(cpoints, rpoints, assemblies, routing files, 3D sketches, and routing templates)

(it is assumed in this section that you are routing piping with elbows and that in your Routing Options, “Save Route Parts Externally” is unchecked and that “Save Route Assembly Externally” is checked For more information on Routing Options, see the next section “Routing Options and Settings” Refer to the “See Also” comment at the end of this section for routing tubing or bent pipe)

Here is the order of operations and how they all work together…

• When you open a new assembly, save it, then insert a component into the assembly that has a Cpoint SolidWorks will prompt you to start a new route by showing the "Route Properties" dialog in the Feature Manager if you have

“Automatically Route on Drop of Flanges/Connectors” selected in your Routing options

See also, Chapter 3 – Starting a New Route

• It is here that you can specify a route assembly file name, the template you wish you use, the Base Pipe Part file you will use for the route, the schedule of pipe, coverings on the pipe, weld gaps, the Elbow Part file you will use, and several other items

• SolidWorks will then insert a new subassembly into the current assembly that is based on the Routing Template you selected, and automatically switch to you editing an in-context 3D Sketch inside that new assembly The component you dropped into the assembly that started your route is automatically moved into the

subassembly by SolidWorks If you were to start your route using a component already in the assembly, that component would not be moved into the routing subassembly This is important to understand Also keep in mind that the component you just placed into your assembly may not have mates assigned to it yet, so it will more than likely need to be mated in place after you edit your route This may also cause your route to move slightly This is why it is important to properly constrain your route sketches while editing One trick is to add “Mate References” to the parts you will used to start your route That way, when you drop them into your assembly, you can snap them to a mating component to lock them into place

• You can add fittings, components, and branches as necessary by dragging and dropping parts onto sketch endpoints or split entity points from the Design Library, and Windows Explorer There are a number of different ways you can

add components to your route We will cover them all in Chapter 4 – Routing Pipe

• Once you are finished sketching the route, exit the sketch, and SolidWorks will populate the route with elbows and create the Virtual Routing Files that correspond to the sizes of pipe you routed in the 3D sketch The default file name

of each of these files is taken from the Pipe Identifier field in the Design Table of the size/type of pipe you routed, the route subassembly name and the top level assembly name

• Those routing files will contain configurations for each length of pipe you routed

The graph at left shows the relationship between the Routing Subassembly file, the base pipe file, the size/type

configurations, and the Routing Files

See also:

Chapter 4 – Routing Pipe Chapter 5 – Routing Tubing

Routing Options and Settings

There are several customizable options and user settings associated with the Routing Package This is a brief explanation of their functions

The Routing Options Page is located on the Tools-Options dialog, under System Options

General Routing Settings

Automatically Route on Drop of Flanges/Connectors

If this box is checked, SolidWorks will start a new route if you drop a part with

routing properties (Cpoints) into an assembly

The component you dropped into the assembly will automatically be moved into the routing subassembly when the route is started This means the part will not be constrained inside the routing subassembly SolidWorks will create a fixed relationship between the routing

subassembly and the top level assembly you started the route in so that the route does not move around randomly It is my recommendation that you add a Mate Reference to the component that you will be starting the route with, so that when you drop it into the assembly, you can snap it in place onto an existing piece of equipment or component

If this box is unchecked, you can drop routing parts into an assembly, and

SolidWorks treats them like any other part without starting a route

If you were to drop a flange onto a vessel nozzle without starting the route so you can add mates to lock the flange into position Then go back and start a new route from the Cpoint on that flange, the new routing subassembly would not contain the flange The route will start from the pipe protruding from the Cpoint on the flange, but will not have the flange in the routing subassembly

Automatically Route on Drop of Clips:

If his box is checked, SolidWorks will automatically try to run your route through the clip whenever one is dropped into a tubing or electrical routing subassembly

In the image below, I started a new assembly and then inserted a Tubing-Male Pipe Weld Connector from the Design Library I then right-clicked on the tubing Cpoint and started a “Flexible” tubing route

With the Option Box UNCHECKED, I then dropped a PClip into the route while I was editing it As you can see by the image below, my route hasn’t changed, except that now

I have a clip inserted into the assembly

If I go back into the Routing Options by selecting “Tools-Options” from the top menu and check the box next to “Automatically Route on Drop of Clips”, and then insert the same clip, the route will attempt to run the tubing through the clip See the image below

This technique also works with orthogonal piping routes and it can also be turned

on or off mid-route as shown above without exiting the route

See Chapter 8, Creating Custom Clips for information on how to make your own hold-downs, u-bolts, clips, etc for use in piping and tubing routes

Always Use Default Document Template For Routes:

If his box is checked, SolidWorks will grey out the option for selecting a Routing Template file when you start a new route (see image below)

Automatically Create Sketch Fillets

As you route your 3D sketch, the filleted corners that the elbows will sit on will be created if this box is checked Otherwise, fillets will not be added to the route automatically, and elbows will not be automatically placed in the route when you exit the sketch This option is not interchangeable during routing Whatever condition this box is in when you start the route, will be applied to the route continuously You cannot start the route without sketch fillets, then exit the route, change the setting, edit the route and expect sketch fillets to be placed

automatically The condition is applied when you start a route, and remains in that condition until you start a new route

Automatically Add Dimensions to Route Stubs:

A Route Stub is a short piece of pipe or tubing that is added to the ends of a routing part when you bring it into a route If this box is checked, SolidWorks will add a dimension defining the length of that stub

The "browse" box is unselectable if the “Always Use Default Document Template For Routes” box is checked This means you are forced to use the template specified under "Routing File Locations"

Enable Route Error Checking:

If this option is checked, SolidWorks will check your route and inform you if your Route Sketch contains an error In the example below, there should be a fillet between the horizontal sketch line and the vertical sketch line to represent an elbow There is not, so SolidWorks denotes an error in the sketch by placing a red circle with an “X” in it inside the feature tree

Shown above: Enable Route Error Checking selected

Shown above: Enable Route Error Checking unselected

Display Error Balloons:

If “Enable Route Error Checking” is selected, then this option becomes available,

if not it is grayed out If this option is checked, then SolidWorks will inspect your route as you draw the sketch lines, and display a notification balloon telling you when there is an error on your sketch line, and give you a recommendation on how to correct it See image below

Include Coverings in the Bill of Materials:

If his box is checked, SolidWorks will add the material covering your route

(insulation, etc) to the Bill of Materials when a drawing is made

Save Route Assembly Externally:

If his box is checked, SolidWorks will create a new assembly file for your route, based on the name and save location used when you started your route This file will not be saved inside the main assembly as a Virtual Component, but instead on your hard drive When you start the route, you will have the ability to specify a location and name of the file

Save Route Parts Externally:

If his box is checked, SolidWorks will create a new pipe part file for your route, based on the “Pipe Identifier” property in the Base Pipe Part file If this option is unchecked, SolidWorks will save the file inside the routing subassembly as a Virtual Component

Use Automatic Naming for Route Parts:

If his box is checked, SolidWorks will automatically name the Routing Part Files when you exit the route based on the Pipe Identifier Property specified in the Base Pipe Part file Otherwise, you will be prompted for the file name and location of the Routing Part File

Use Triad to Position and Orient Components:

If his box is checked, SolidWorks will display a

“Triad” or “Positioning Orb” to rotate and move the component after you drop it into your route

Use Centerline Dimension:

Checking this box will tell SolidWorks to dimension your route from the Centerline

of the pipe when dimensioning it to other components or surfaces in the routing subassembly In the image below, “Use Centerline Dimension” is left unchecked, and SolidWorks created the dimension from the wall to the nearest outside surface of the pipe, not the centerline

When you are editing the route and place a dimension, you can switch to the

“Other” tab and change the setting on the fly If you created the route with insulation and check the box marked “Include covering thickness” then SolidWorks will dimension to the outside of the insulation instead

Component Rotation Increment (degrees):

This value determines the increments that a part will be rotated when you drag a component onto your route, and hold down the shift key, and a left or right arrow key before letting go of the left mouse button

or

Pressing the above combination of keys will rotate your component before you drop it when you drag it onto a point in your route

Text Size for Connection and Route Points:

This number is the font height of the text for connection and route points If the slider is to the far left, the text is very small, but you can still select the CPoint and Rpoints

The image below left shows the result of the slider set at 1, the image below right shows value set to 10

Piping / Tubing

Create Custom Fittings:

If this box is checked, SolidWorks will allow the creation of custom elbow files if

“Use Elbows” is checked in the Route Properties, and you have an elbow angle

in your route that cannot be found under the “BendAngle@ElbowArc” dimension name in the elbow’s design table that matches that size of pipe

The image below shows a route using 60 degree custom elbows

If your company standards do not permit the use of custom elbows, then this box should be left unchecked I recommend leaving this option unchecked, as sometimes you could end up with an 89.9 degree elbow by accident in your BOM

See Chapter 4 – Creating Custom Elbows, for more information on creating

custom elbows when you exit the routing sketch

Create Pipes On Open Line Segments:

If this box is checked, SolidWorks will generate pipe for 3D sketch segments that have fittings at only one end

For example, if this is unchecked, and your sketch segment is connected

to a flange at one end, and is open on the other, no pipe will be generated on that segment

The image at right shows a typical piping segment while in the 3D sketch Regardless of the option box being checked, the pipe shows as it is drawn in the sketch

When you exit the 3D sketch, the effects of the option box being checked or unchecked are displayed

The image below left shows the effects of having the option box checked, and creating a route where pipe has been created on an open line segment

The image below right shows what happens if the option box is unchecked and a route is created on an open line segment

Route created with box checked Route created with box unchecked

This option will only work if there are at least two components in a route If there is only one part in the route, then the pipe will always be displayed

If an elbow, or a bend is added after a component, a pipe segment with an open line segment will display the pipe after exiting the 3D sketch regardless of the status of the check box See image below

The image above is taken from a route where the option box was left

“unchecked”

Electrical Cabling

Enable Minimum Bend Radius Check for Cables:

This option box is only used for routing electrical cables For routing flexible tubing, this option is located in the Route Properties panel when you start a new flexible tubing route

Enable Minimum Bend Radius Check for Wires:

This option box is only used for routing electrical cables It will report an error if the bend radius for individual wires inside a harness is too small

If you start a route with the option checked, and decide later that you would

rather leave it unchecked, you cannot make the switch in the middle of the

route

Routing File Locations

These paths tell SolidWorks where to find the components that will be used in your routing subassemblies It is HIGHLY recommended that you place ALL the components to be used in these path locations, or SolidWorks may get confused, and load the incorrect parts

(Also see Chapter 3 – The Design Library & Chapter 13 – Using the Routing Library Manager)

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Chapter 2 – Required Features of

Components

Cpoints & Rpoints

Almost every part used in a piping or tubing route must have some sort of identifier that tells SolidWorks that it is part of the Routing package That is the function of the Cpoints and Rpoints

Cpoints are Connection Points that tell SolidWorks where to start a piece of pipe or tube

from They also contain routing properties that tell SolidWorks what size of pipe/tubing

to route The Cpoint can be designated as a Fabricated Pipe, Tube or an Electrical Connection Point Electrical Connection Points are not covered in this Piping & Tubing manual; please refer to the SolidWorks documentation for more information on routing electrical components

Rpoints are Routing Points that are used to locate the component on a point in the 3D

Sketch These points can be the end point of a line, or a “Split Point” in the sketch

Rpoint (placement of component)

Cpoint (size, type & starting point of pipe/tube)

Cpoints and Rpoints are added at the “Part” level and are created on top of existing sketch points, sketch line endpoints, or the origin

Pipe Between Cpoints

Reducer Located

Using Rpoint

Let’s walk through adding a Connection Point to a buttwelded valve Open the file CH02-4inBW-Valve.sldprt and follow the steps below

1 To place a Cpoint, select the point that you want it placed on top of, and then control-select a face on the part that is facing perpendicular to the direction you want the pipe to run

Sketch Point

Face

2 From the “Routing” toolbar,

select “Connection Point”

I like to create a sketch, at the

very end of my feature The

plane I use runs through the

center of my part, so my sketch

is in the middle of my part too

Then I add 2 sketch points

where I want my Cpoints to be

3 The Feature tree will now display the

properties for the new Cpoint In the Connection Point properties area, set whether you want this Cpoint to be a Piping

or Tubing Cpoint

Select Fabricated Pipe

4 Set the Nominal Size of tubing or pipe that

you wish this Cpoint to represent (you can

have multiple configurations in a part to have multiple Cpoint pipe/tubing sizes)

Enter the Nominal Pipe Size Here

5 If you wish to make this Cpoint follow a

specific property, enter it here

For example, let’s say that this valve HAS

to be connected to a Stainless Steel Flange In your flange part file, you would add a column in the design table that would

be called “$prp@Specification” and only flanges or pipe that have Stainless Steel in that column would be allowed to connect to this Cpoint This step is completely

optional, no value is required

At my company, we have 23 different specifications Each specification determines what class of flange to use, wall thickness

of pipe, material, etc So my pipe & elbow files have the specification names for each type of pipe or elbow For example, a typical specification name for me is S600-A We name our

configurations in the pipe file 1” S600-A, 2” S600-A, and so on

The Material for that specification is always ASTM A312 TP304

Having the specification name in the Specification column of the design table will tell SW to only offer us the sizes that match the specification name of the Cpoint So any pipe I route on that spool will always be ASTM A312 TP304

6 Select Okay to insert Cpoint1 into the Feature Tree

7 Repeat steps 1-6 to create Cpoint2 on the other side of the valve

8 To add the Rpoint, select the “Origin” and then select “Route Point” from the Routing toolbar

Origin

9 There are no options to set, so select Okay to insert Rpoint1 into the Feature Tree

10 The valve should now contain 2 Cpoints and 1 Rpoint You can now insert the valve onto the endpoint of a routing line, or onto the sketch entity of a routing line such as a Split Point

Pipe (Base Pipe Part File)

You can open the “Pipe-Astm-A53.sldprt” file provided that I created for these examples, and compare my part to yours if you have questions

SolidWorks uses a Base Pipe part file that contains all of the required information to route piping You specify the pipe file and the configuration you wish to use when you first start your route SolidWorks then uses the information in that configuration to

display the route and create the routing files when you exit the 3D sketch

All Base Pipe part files must contain the following:

PipeSketch

The part file must contain a sketch named PipeSketch, consisting of two

concentric circles with dimensions named OuterDiameter and InnerDiameter

The sketch plane for “PipeSketch” must be placed the “Front” plane and the center of the circle must be constrained to the origin

You should keep everything exactly like I have it shown in these steps Make sure that when you name features, sketches, and dimension names, that you type in EXACTLY what I have shown here

For example, naming the sketch with the 2 concentric circles

”Pipesketch” is a lot different from naming it “PipeSketch”

Also, do not add spaces between words if I don’t show them Again,

“Pipe Sketch” is not the same as “PipeSketch”

The design table, and Routing software will look for specifics This isn’t a game of horse-shoe people, close doesn’t cut the mustard

Sketch named “PipeSketch” in a feature

Extrusion

An extruded feature of the sketch named “PipeSketch” with an extrusion

dimension named “Length” Don’t forget to rename the Extrusion feature to

“Extrusion”

Extruded “PipeSketch” named “Extrusion”

To rename the sketch dimension, select

it, and then type the new name here

Do not change the “@PipeSketch” text, just the text in front of it

Rename the Extrusion Dimension to

“Length@Extrusion”