In this post, we’ll show you how to prepare models so you can use them as Routing components.
SOLIDWORKS Routing has many hidden tricks, features and requirements.
Our goal is to collect all of them in this post.
This post will be a constant work-in-progress, so please let us know if you have something to add, if it lacks crucial info or if it contains a mistake.
For more general information about the SOLIDWORKS Routing add-in, check out our article How to create a Routing library from scratch.
This article started out as a section in the routing library post, but it quickly became large enough to warrant its own post.
Pipes are incredibly easy, compared to flanges and tees. The rules are documented and clear.
But these rules are very strict.
More info in the official SOLIDWORKS help:
Our other article has a section on how to use the new pipe file by adding it to the database.
You can use any part or assembly as routing components in a routing assembly.
But you need to add a few features to the model first. Click them to go to the correct section.
You can do this in two ways:
A Connection Point or CPoint defines where the pipe, tubing or cable starts or ends.
It is a feature in the feature tree. You can only edit this feature when the Routing add-in is enabled.
Connection points are for parts, Assembly Connection Points are for assemblies.
When you add a flange to an existing piece of pipe, the flange connects at the connection point. If the diameter and schedule match.
It has a position and a pipe direction. You can see where SOLIDWORKS adds the connection point to a welding neck flange in the image below, exactly at the connecting face between pipe and flange.
A fitting needs a connection point for every port, so a flange needs one CPoint and a tee needs three CPoints.
A unique thing I found is that SOLIDWORKS always names the first point CPoint1, even if you deleted one previously. Normally it just increases the count, it never reuses a number.
There are a few important properties that you need to set here. For piping, you need to set at least these:
You only need the Port id if you read in P&ID files automatically.
Forum topic on schedules and the importance of the CPoint properties.
A Route Point or RPoint defines the position where you add the component to the existing 3D sketch.
Just like the CPoint, it’s a feature in the feature tree. You can only edit this feature when the Routing add-in is enabled.
Route points are for parts, Assembly Route Points are for assemblies.
It is a much simpler feature than the CPoint and has only one parameter, its position.
For a welding neck flange, like in the image below, it makes sense to have the route point at the connecting face.
When you add the flange to a route, the route will become a little longer because the flange snaps in place at the connection point.
You need one RPoint per routing component. Only excentric reducers need zero.
For a flange, this marks the end of the pipe.
For a tee or elbow, the route point marks the intersection of the ports.
For flanges at least, you need to create two reference axes:
SolidWorks looks for these names and the names are probably case sensitive. We could not find clear proof, the best we could find is this help article.
Mate references are a great way to make parts snap in place when you drag them into an assembly. This is a good introduction video and it’s only 4 minutes long.
You say which edges and faces are important, define the alignment and then give the mate reference a name.
If you define mate references on one part like we do on our fasteners, you can easily drag parts into a hole in another part and SOLIDWORKS will add one or two mates.
When you define mate references on two parts that should always go together, you need to give the mate references the same name. You also need to define the faces in the same order.
Mate references are not mandatory for routing parts, but they are very useful.
When you create a new route (and thus a new subassembly) by dragging in a flange, the flange will snap to an existing flange. SOLIDWORKS then adds a few mates, instead of making the new subassembly fixed.
We have found two mate reference types in the default library. You should use these names to make all parts work together.
Multiple configurations are pretty much required for routing components to work well.
When you add a flange (or any other component) to an assembly, SOLIDWORKS searches through all configurations within the new file.
It then tries to match:
Configuration names are very important, it seems. According to this forum post, SOLIDWORKS searches the configuration name for sizes and schedules.
I cannot confirm this yet, but this setting in the Route Properties tab hints at such functionality.
For those of you that don’t know; a design table is an Excel file. The table is stored within a SOLIDWORKS file and contains a row for each configuration in a model.
You can control dimensions, equations, colors and custom properties, you can even suppress features. You can read all about them in the help.
Routing relies heavily on design tables. All routing files that SOLIDWORKS ships with the software have a design table.
Custom properties are controlled via “[email protected]”.
When you go through the Routing Component Wizard, this cryptic screen is the second to last step.
The menu on the left is called Component Attributes, but these are actually custom properties.
The top section contains configuration-specific custom properties, the bottom section contains custom properties for the entire file.
SOLIDWORKS adds these custom properties to your file when you click Finish, but:
We could not find a complete list of the requirements for routing components.
But now there is one. We were able to get our own flanges working and we wrote all the crucial pieces of information down here.
Also check out our other post on routing: How to create a Routing library from scratch
We hope it was helpful for you as well. Please let us know if you have something to add.