Create Connectors 

The Build Connector command can be used to add connectors to a part that is unique - meaning it has one reference and one instance only.

The Manage Connectors dialog box will list all connectors on the selected part. To see a connector and its associated geometry on the part, select a connector from the list.

Adding a connector is explained below; Delete, Modify and Duplicate are explained elsewhere in this section. To Publish a connector means you are allowing people who do not have write access to your document to establish a connection. This is explained further in Using Work Packages. You can Publish or Unpublish connectors using the two buttons.

Select the type of connector - piping, HVAC, etc.

In some applications the flow direction field will be available. The piping (or tubing) part connector has flow direction built in and you must select a flow direction also from the drop down menu. The mechanical part connector has no flow direction. 

Another type of connector - the nozzle connector - will be available if you are placing a connector on a nozzle. A nozzle connector must be placed on the end of the nozzle that connects to equipment. A part connector is placed on the end that connects to the pipe or duct. 

An electrical part connector should only be placed on a socket. The electrical part connector should be placed on the end of the socket that connects to equipment. A cableway part connector should be placed on the free end of the socket that does not connect to equipment.

When you are placing a connector on a Bendable, such as a bendable pipe,  you must use the Define New Geometry option. You must not use existing geometry to place the connector.

You can name each connector by selecting in the Name field. This is useful for some functions, such as designing using a schematic. See Customizing 2D and 3D Connector Names for more information.

The concept of Publishing or Unpublishing a connector is explained above. Check the checkbox as necessary.

Face, orientation and alignment are explained below.

The face is generally defined using a face of the part, such as the end of a pipe. Alignment is usually defined using a line, such as the not-shown line along the centerline of a pipe. Orientation is defined using the xy plane, or another plane or face to define an "up" direction.

In the illustration below the Z axis indicates the alignment of the connector. It also indicates the direction in which routing will occur.  The X and Y axis together define the orientation. They are useful when attaching two resources. 

It is necessary to select geometry in the part to which you want to attach a connector so that these three characteristics are correctly defined. If the part does not have the necessary geometry then you must create it.

Click the Select Face button to select a face. Selectable faces will highlight as you move your pointer over the part.

Click this button to select the alignment. You will only be able to indicate the alignment by selecting a line -  from the construction geometry, or elsewhere in the part if there is one. You can only select a line that is perpendicular to the face plane.

Click this button to select the orientation. You will only be able to select a plane that is perpendicular to the face you selected. If you cannot find a plane to select, click the Swap Visible Space button (see below) to make the construction geometry visible, and select a plane.

Some connector types require you to place a datum point. The datum point is placed by clicking this button and then clicking a 3-D point on the part. The datum point is used as follows:

• Lofted reservation section: Datum is used to define where the spline will start and end when creating lofted reservations.
• Hangers: See Hanger Design documentation.
• All applications with flexibles: The datum point is placed in two situations: (1) Datum is used to define where the spline will start and end when creating flexible tubes. (2) It is recommended that you place a datum point on each part connector to which a flexible may be routed. This is needed to allow a flexible to update when you move a part in a design.

You can display the part construction geometry, if there is any, to make it easier to select existing geometry. Do this by:

• Right click on the part entry in the specifications tree.
• Click Hide/Show. The part will disappear from the screen.
• Click the Swap Visible Space button . The part will reappear on your screen with the construction geometry visible. Clicking the button again will toggle you back.

Select a type.

For Flow direction, select In, Out, InOut or None.

Select the Face type.  A Hole connection allows a routable to pass through it - it is useful for placing parts like clamps along a run without cutting a tube. A Face connection will stop a routable and not allow it to pass through.

Select an alignment.

Choose an orientation: Circular will allow the connector to attach to another connector at any orientation; round ducts and pipes, for instance, do not need a well-defined "up" direction because they can rotate. A Rectangular orientation is used for parts like rectangular ducts; they do not have a strict ''up" direction. Up allows the connector to attach to another connector or part in the up position: horizontal trays, for instance, require a well-defined "up" position. You can also use the "up" orientation for a hole connector. In the image below, the connector on the right has the up orientation, the connector on the left does not.

The number in the Number field is assigned by the application. This can be significant because when you are creating a new connector, you have the option of using the alignment and orientation used in the previous connector after you select the face. You can choose to do this, or select a new alignment and/or orientation.

Click the Define Plane button to redefine the plane as well as the origin by clicking once on the face.

Click the Define Plane using Compass button to redefine the plane using the compass.

Click the Define 3-point Plane button to define the plane by clicking on any three points with your pointer. The connector will be placed on the first point you click.

Click the Define Line-Point Plane button to select the plane by clicking on a point and a line, like an edge. The connector will be placed on the first point you click.

Click the Define Line-Line button to select the plane by clicking on two lines. The plane will be defined by the first line selected. But if the two lines are parallel the plane will be defined as the plane in which both lines exist.

Click the Define plane at center of circle  button to select the plane by clicking three points on the edge of a circle. This method is used for multi-CAD documents, usually for CGR circles. You can click at points where two lines meet or in the center of a face.  The Z axis of the plane manipulator will be placed according to the right hand rule. If you click clockwise the Z axis  will point into the object. If you click counter clockwise the Z axis will point out from the object.

Click the Define plane at product origin  button and then the object to place the plane manipulator on the origin of the object. The plane manipulator axis will match that of the product.

  Click the Define Orientation button to change the orientation. Click the button and then click a point or a line. If you click a point the X axis will point to it. If you click a line the X axis will become parallel to the line. 

Use the Move Origin buttons to define the plane. Define Origin at Plane or Compass allows you to define the origin using the compass or plane command. You use the compass or plane as the base plane along which the origin can be selected. Define Origin at Point or Center of Face lets you select the origin by clicking on a point or face. Define Origin at Center of Circle allows to select the origin by clicking at three points - the origin will be placed in the center of an imaginary circle drawn using those three points. The plane and orientation will not change when using this command.