SOLIDWORKS Routing 101: Pipe Design

Article by Zach Brown on Nov 10, 2021

In this blog, we will explore the basics of SOLIDWORKS Routing for Pipe Design. In this tutorial, we will cover the following topics:

  • How to turn on the SOLIDWORKS Routing add-in
  • How to access the Routing Library
  • How to start a Pipe Route using Flanges
  • Overview of Routing PropertyManager
  • How to create a SOLIDWORKS Drawing of the Pipe Route.
  • How to edit the Route and manipulate 3D Sketches
  • How to add Flanges, Straight T, and Valves to complete the design
  • Separate the design for shipping by placing Flanges where spools will be taken apart, and use the Spool Feature to group the components accordingly.

How To Turn On The SOLIDWORKS Routing Add-in

Go to Tools > Add-ins, check the box for SOLIDWORKS Routing on the Active side. Checking the box on Start Up side will cause the Routing add-in to load when SOLIDWORKS is launched.

SOLIDWORKS Routing Add-in

How To Access Routing Design Library

The SOLIDWORKS Design Library is located in the SOLIDWORKS Task Pane. Expand the Design Library folder to see the Routing subfolder. Located below the Routing folder, the Piping folder includes all components needed to create the Piping Route.

How to Access SOLIDWORKS Routing Design Library

Note: If you do not see the Design Library, go to Tools > Options > System Options > File locations > Routing, and click the Add button. The default folder for the Design Library is C\ProgramData\SOLIDWORKS\SOLIDWORKS 20XX\Design Library.

SOLIDWORKS Routing Design Library Accession System Options

Starting A Piping Route

  1. For this tutorial, we will begin by opening a new assembly in SOLIDWORKS
  2. Next, browse to the Flanges folder under the Piping folder in the Design Library
  3. Drag the slip on weld flange from the Design Library to the Origin of the assembly
  4. Select the configuration Slip On Flange 150-NPS6 and click OK
  5. After clicking OK, the Route Property Manager is displayed in the Design Manager Feature Tree.

    Starting a Piping Route in SOLIDWORKS

 Route PropertyManager Overview

  1. File Names > Routing Subassembly shows the nomenclature for the Routing Subassembly that will be created.
  2. Under the Pipe Category, you can select Use Weld Gaps if you would like to add a gap between components.
  3. The Use Standard Length option will divide the pipe into standard purchased lengths. So, if you buy pipe in 20ft lengths it will divide the pipe into 20ft sections.
  4. Under Bends – Elbows, set the option to Always use elbows. For this tutorial, we are using a 90deg short radius elbow. You can click the browse button to find the component. Click OK in the Route PropertyManager.

    SOLIDWORKS Route PropertyManager Overview

Creating The Pipe Route

Once you click OK in the Piping PropertyManager, you will see a new Routing Subassembly in your Feature Tree. You will also notice that a 3D Sketch has been placed at the origin of the flange. The 3D Sketch is the path the pipe will be swept along.

Create a Pipe Route in SOLIDWORKS

  1. On the Piping Toolbar or Sketch Toolbar choose the Line Tool. Start the next line at the endpoint of the 3D sketch. Drag the Line upwards and click the second point.
    • If the line is not going in the right direction, you can toggle the direction by hitting the Tab key. This changes the orientation of the sketch from YZ, to ZX, to XY.

      SOLIDWORKS Pipe Route

  2. After you place the line, an elbow is placed to join the pipe. The radius is determined by the elbow chosen in the Routing PropertyManager. 
  3. Continue adding lines. Dimension each segment by clicking Smart Dimension and selecting a line segment. The dimension goes to virtual sharp of radius if there is a change in direction of the pipe.

    Smart Dimensions for SOLIDWORKS Routing

  4. You can delete a radius to remove the elbow.

    Sketcher Confirm Delete Window in SOLIDWORKS

  5. Click the Line Tool again and add the lines shown below, then we will add a straight tee to the junction.

    Line Tool in SOLIDWORKS Routing

  6. Drag a straight tee from the Piping Library, Tees folder to the junction and select OK for the default configuration. Notice the tee snaps to the correct orientation based on the 3D Sketch.

    SOLIDWORKS Piping Library Tees Folder

  7. Drag another straight tee from the Piping Library, Tees folder to this area of the Pipe Route. If the Tee is not orientated correctly, hit the Tab key on your keyboard to flip orientation. Click to place tee, then click OK for the configuration. Notice a 3D Sketch line now coming from the tee.

    SOLIDWORKS Routing Straight Tee Inch

  8. Delete the sketch line coming from the elbow, then drag the line endpoint (coming from the tee), to the endpoint of the line where we deleted the radius. Then close the sketch in the Confirmation Corner. SOLIDWORKS Confirmation Corner Symbol


    SOLIDWORKS Routing 101

Note: Section view shows how components are created when the Pipe Route is finished.

Complete Pipe Route in SOLIDWORKS

How To Edit the Route

  1. To edit the route, right-click on the Routing Subassembly and choose Edit Route, or choose Edit Route on the Piping Toolbar.

    How to Edit Routes in SOLIDWORKS

Edit Pipe Route and Adding Valves

  1. Drag a gate valve from the Piping, Valves folder and drop it on a sketch line. Again, the Tab key controls the orientation of the valve.

    How to Edit Pipe Routes in SOLIDWORKS

  2. Click No to shorten the length of the pipe between the Pipe Nipple and fitting.

    Adding Valves for SOLIDWORKS Routing

  3. Drag over two more gate valves. Click No to shorten the length for each.

    Gate Valves in SOLIDWORKS Routing

  4. Right-click on a gate valve face and choose Move Fitting with Triad.

    SOLIDWORKS move Fitting with Triad Option

  5. We can rotate the valve at any desired angle using the Triad Wheels.

    SOLIDWORKS Routing Trial Wheels

  6. Drag over two more straight tees from the Piping, Tees folder.

    Piping Tees in SOLIDWORKS

  7. Add a line in the ZX direction (Tab key for orientation) to both tee sketches.

    Tee Sketch Orientation for SOLIDWORKS Routing

  8. We can add a Construction Line between the two endpoints, then apply an Along Z relationship to line them up. Finish adding dimensions to the sketches as desired.

    Along Z for Construction SOLIDWORKS Routing

  9. To finish up the design, drag over two slip on weld flanges to the ends of each sketch. Choose Ok to the default configuration.

    SOLIDWORKS Routing Slip on weld flanges

  10. Notice the two folders in the Feature Tree. The Components folder contains all the flanges, valves, tees, etc. The Route Parts folder contains all piping components.

     SOLIDWORKS Routing Feature Tree Components

Using The Spool Feature to Separate Design

After the Pipe Route is complete, we can use the Spool Feature to separate the design into smaller, shippable spools.

For this exercise, we will split the design up into three smaller segments. First, we need to drag over some slip on flanges where we want to break up the design.

SOLIDWORKS Spool Feature

  1. Drag over another slip on flange and line it up with the previous flange. Watch for the Cursor Feedback that indicates the flanges will be connected, then release the mouse button.

    SOLIDWORKS Routing 101 Cursor Feedback

  2. Add flanges in the same manner to two other locations on the spool.

    Add Flanges in SOLIDWORKS

  3. We can right-click on one of the pipes between the valve and the segment and choose Remove Pipe.

    Remove Pipe Option in SOLIDWORKS

  4. The pipe is removed and the flanges move next to the valve. Do this for the other pipe between the flange and valve as well.

    Remove Pipe SOLIDWORKS Routing

  5. Before we define the segments with the Spool Feature, we can set up the naming convention for the spools. Go to Tools > Options > System Options > Routing > Spool name format.

    SOLIDWORKS System Options - Routing Spool Name Format

  6. To define the spool segments, right-click on the Routing Subassembly, and choose Define Spools.

    SOLIDWORKS Routing Define Spools Option

  7. In the Spools PropertyManager, you can change the name of the Spool and define a color. Click the Push Pin to keep the dialog up after clicking OK
  8. For Spool Segments, click one of the line segments at the beginning of the route. In the Spool Components section, it will add the components for the segment. 
  9. Click OK.

    Spool Components and Segments in SOLIDWORKS

  10. Change the color and name of the second Spool. For Spool Segments, we have chosen all sketch lines in this segment, because of the junction where the pipe splits at the tee. 

    SOLIDWORKS Spool Segments

  11. Change the color and name of the third Spool. Select all the line segments highlighted in magenta below, then click OK and unpin the PropertyManager.

    SOLIDWORKS Routing Spool Segments

  12. Each Spool is located in a folder under the Routing Subassembly. If you need to edit a segment, right-click on the folder and choose Edit Spool.

    SOLIDWORKS Edit Spool Option

Creating A Spool Drawing

We can use the Pipe Drawing command to quickly create a drawing with multiple sheets, drawing views, BOM’s, and balloons.  

  1. In the main assembly, preselect the Routing Subassembly, and choose Pipe Drawing from the Piping Toolbar.

    How to Create  a Spool Drawing in SOLIDWORKS

  2. In the SPOOL Drawing PropertyManager, select the three spools under Spool Selection.
  3. Choose a Drawing template, Sheet format, and Piping BOM template.
  4. Select Include auto balloons.
  5. Choose View on separate sheet. This will place each spool on a separate sheet.
  6. You can choose to Show route sketch or unselect to hide the sketches.
  7. Click OK.

    SPOOL Drawing Options in SOLIDWORKS

  8. A drawing is generated with a sheet for each spool, along with balloons and BOM’s.

    SOLIDWORKS Spool, Balloons, and BOMS

Cleaning Up the Drawing

For the remainder of this tutorial, we will look at a couple of tools to quickly clean up this drawing.

  1. On the Annotations Toolbar, choose Magnetic Line. Drag the Magnetic Line through a set of balloons. The balloons snap to the line. The Magnetic Line can be dragged around and the balloons will stay attached to the line.

    Cleaning up Drawings for SOLIDWORKS Routing

  2. On the Annotations Toolbar, choose Centerline. Click on each pipe to add Centerlines.

    SOLIDWORKS Annotations Toolbar Centerline Option

  3. Let's add a sheet to show a view of the whole spool assembly. Click Add Sheet button next to Sheet3.

    SOLIDWORKS Add Sheet Option

  4. On the Task Pane, click the View Palette tab. Use the pulldown arrow to choose the top-level assembly, or click the browse button and browse to assembly. Drag over a Trimetric view. Adjust drawing view scale as necessary.

    SOLIDWORKS Routing Task Pane View Pallet

  5. Rename Sheet4 to Sheet00 and drag the sheet tab to a position before Sheet1.

    View Pallet SOLIDWORKS Routing

  6. Define the Spool Segments. From the Annotations Toolbar, select the Balloon command. 
  7. Under Settings, choose Inspection for the Border style, set to 5 Characters, and under Balloon text, choose Spool reference.
  8. Click the edge of a pipe in a spool segment to place the balloon. The balloon shows the spool name. 

    SOLIDWORKS Routing Settings

  9. Let's create a new Style for this balloon so we can use it again. Highlight the balloon. In the Balloon PropertyManager, under Style, click Add or update a style.
  10. Give the Style a name and click OK.

    SOLIDWORKS Flag Note Bank

  11. We can use the new style to create additional balloons with spool names. Click the Balloon command, and under Style, use the drop-down to choose the Style we added.
  12. Place the additional balloons by selecting a pipe edge in each renaming spool segment. Balloons are added in the same style with each spool reference. 

    SOLIDWORKS Balloons Pipe Spool Style

  13. Finally, let's rename each sheet to match the spool name. Right-click on a sheet in the Drawing PropertyManager and click Properties. Under Name, type in the name of the spool segment and click Apply Changes. Repeat for remaining sheets.

    SOLIDWORKS Routing Piping Sheet Properties

Want to become an expert? 

Take the official SOLIDWORKS Routing: Piping and tubing course from GoEngineer. 

GoEngineer Professional SOLIDWORKS Training Routing: Piping and Tubing

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About Zach Brown

Zach Brown is a certified SOLIDWORKS Expert and a Technical Support Engineer. Prior to working at GoEngineer, he spent 15 years as a mechanical designer, CAD support tech, and instructor using SOLIDWORKS. His hobbies include playing guitar, riding motorcycles, and skiing.

View all posts by Zach Brown