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The Content Center Library contains libraries of standard and custom Autodesk^® Inventor^® parts (fasteners, steel shapes, shaft parts) and features. It includes standard conduit parts (hoses, pipes, tubes) and tube and pipe fittings (couplings, elbows, flanges, tees, and so on) for tube and pipe systems. You can place these components into assemblies using AutoDrop.

The components comply with industry standards, and libraries from several different industry standards are provided.

The Content Center in Autodesk Inventor provides the means to access and maintain libraries. You can create as many libraries as you need on the Autodesk^® Vault Server. You attach them to the Content Center using the Configure Content Center Libraries command.

If the library has not been attached to the Autodesk Vault Server, attach it first.

You access the library parts using the Place from Content Center and Replace from Content Center commands. After you locate a part in a library, you set parameters for the part. Then use AutoDrop to insert the part in the assembly file or directly onto a run. When a library part is dropped into an assembly, an .ipt file is created for it. The inserted part is added to the Model browser.

To manage libraries on the server, click Start Programs Autodesk Autodesk Data ManagementAutodesk Data Management Server Console 2013. Log in to the server, and click OK. Once the console is open, you can perform several operations.

For Tube & Pipe specific libraries, you can manage them the same as you do with Inventor-specific libraries. For example, to reuse custom library parts that you published in earlier versions of Autodesk Inventor Routed Systems, you can import the appropriate library database files. Using the Publish Part command, you can add your own tube and pipe parts that have been authored to the Content Center libraries for standard use.

Autodesk Inventor^® Routed Systems provides three components to manage libraries, configure libraries, and edit library content with varied functions:

Autodesk Vault server

To use libraries in the Content Center, the server must be installed. You can create new libraries on the server and then use Configure Content Center Libraries to attach it to the Content Center. You can permanently delete a library from the server after you detach it from the Content Center.

Configure Content Center Libraries

Attach the libraries on the server to the Content Center.

Content Center Editor

Edit library parts from within the Content Center.

To configure Content Center Libraries for use in a project, open Autodesk Inventor Routed Systems and click Manage Projects.

Using the Configure Content Center Libraries command you can:

• Add new libraries.
• Import Inventor libraries and the Tube & Pipe Library from previous versions.
• Edit or remove existing custom libraries in the Libraries list.
• Update the libraries in the list.

Typically the prerequisite for configuring libraries in the Content Center is that the libraries must exist on the server. Importing libraries to the Content Center is an exception:

• If the target library is a pair of .mdf and .ldf files, start the Autodesk Data Management Server Console. Right-click Libraries in the Admin Tools browser and select Import Library.
• If the target library is a .mdb file, start the Configure Content Center Libraries command. Click Import Library.

Both conduit parts and fittings can be placed into a tube and pipe assembly from the Content Center using AutoDrop.

The following commands are available to locate tube and pipe library parts:

• Place from Content Center directly places library parts. For detailed instructions, see AutoDrop for Library Parts in Chapter 6.
• To replace an existing fitting or all instances in the same fitting type, right-click the fitting to replace and start Replace from Content Center. For detailed instructions, see Replacement Fittings in Chapter 6.

The Content Center offers functionality such as queries and dropping conduit parts and fittings. To take advantage of it, publish custom tube and pipe iParts and normal parts to the Content Center. Custom parts in the Content Center can be shared in multiple projects. It is not necessary to save the same custom parts for each project workspace.

Read/write permissions are required to publish parts to a library. If you need permissions, request them from your system administrator.

Publishing parts automatically points to the default category in which they must be published in the active library. If you click into another category, click the default category in the library tree again to continue the publishing.

To author and publish in Autodesk^® Inventor^®, you use two commands in sequence:

• Tube & Pipe Authoring
• Publish Part

First you create a custom fitting or component and transform it to an iPart factory. Then use the Tube & Pipe Authoring command to prepare the part for publishing to the Content Center. You can also author and publish a normal part (not an iPart) as a fitting.

You can author and publish tube and pipe iParts as either pipes or fittings, but can only author and publish normal parts as fittings.

When you author tube and pipe iParts, you specify:

• Part type
• Connection number
• End treatment of each connection
• Parameter and iPart table mapping
• Connection point and connection axis
• Gender (female, male, or neutral)
• Engagement of each connection
• ISOGEN properties for fittings
• Mating point and pipe axis (for branch fitting only)
• Cut options (for branch fitting only)

When you author normal parts, you specify all the previous items, except for the Parameter and iPart table mapping. In its place, you specify a fixed nominal size.

The Tube & Pipe Authoring command is available as soon as you have an iPart or a normal part file open.

In the Tube & Pipe Authoring dialog box, specify the: .

• Part type
• Number of connections
• End treatment
• Required part parameters
• Engagement
• Optional ISOGEN properties for tube and pipe iParts or normal parts being authored

Once authored, you can publish them to the Content Center. If you do not want to make the part available from the library, you can save the part to a different location.

When creating the iPart, include the necessary values in the iPart table. We recommend that you learn what parameters are required to author tube and pipe parts. You can then create appropriate parameters and features when transforming the part to an iPart factory.

When a sample tube and pipe iPart is open:

• Use the Parameters command to verify the model parameters and user parameters that are used in the iPart. We recommend that you use model equations to define the part parameters. Then multiple part occurrences specified in the iPart Authoring table can update dynamically in proportion.
• Double-click Table in the Model browser to open the iPart Author table. Verify all part occurrences that are defined for the iPart. Each row in the iPart Author table represents a part occurrence for the part family to publish to the Content Center.
• You can customize the pipe length of a part you placed previously from the Content Center. Specify it as Custom Parameter Column in the iPart Author table before you author. Click the column head to select the entire column, right-click, and then select Custom Parameter Column.
• Each row in the iPart Author table can have its own material definition. When needed materials for an iPart are not available in the Materials Library, routes and runs using this material cannot be properly populated. Access the Materials Library to add new or custom materials to the library.

Each iPart Author table has a default row. The default row determines the library part that displays when you open a part family in the Content Center.

For instance, open the sample pipe iPart Autodesk\Inventor Professional <version>\Tutorial Files\Tube & Pipe\Example_iparts\pipe.ipt. In the Model browser, double-click Table to open the iPart Author dialog box:

The row highlighted in green is the default row. To change the default row, right-click the appropriate row number, such as 1/2, and select Set As Default Row. Click OK and the pipe part in the graphics window automatically updates.

The pipe iPart is published to the Content Center. Now when yhou open the part family, the preview image shows the part with parameters in the default row.

You can open 90-degree elbow and 45-degree elbow to verify their default rows on the iPart Author dialog box.

An iPart can have up to nine keys used to define criteria for AutoDrop and filtering out the iPart for tube and pipe styles.

Pipe iParts typically have three family key columns: nominal size, schedule number, and pipe length. For the sample pipe iPart:

• On the Other tab, NPS is primary key {1} and SCH is secondary key {2} .
• On the Parameters tab, PL is tertiary key {3} .

Fitting iParts typically have one family key column: nominal size. For the sample elbow iParts, on the Other tab, NPS is primary key {1}.

The following image illustrates the relationship between iPart family key columns and part family thumbnail page in the Content Center.

Family key columns play an important role in the file naming schema for part families in the Content Center. After authoring and publishing, the sequential combinations of hierarchical keys form the value of the pre-defined property in the Content Center. In this case, {DESIGNATION} is pipe {NS} {SN} {PL}, in which pipe indicates the conduit part type.

The Tube & Pipe Authoring command predefines a list of available part types to author, such as Tubes, Pipes, Hoses, Couplings, Elbows, and Tees. When no category is appropriate for the fitting part being authored, select Other.

You cannot select an edge next to a torus or spline face to define connection points and connection axes.

The Content Center setting defines the library where you want the part to belong. Parts can only be published to libraries that have Read/Write permission. Otherwise, go to your system administrator to request permissions.

When publishing parts, iParts, or features, the Content Center automatically points to the default root category where you must publish the part. Create appropriate subcategories. Then specify the family properties and category parameters so the published parts or features can be queried at a later time.

You cannot add a new library to the Content Center during the publishing process. Use the Autodesk Vault server and Configure Content Center Libraries command to create and attach the library to the Content Center beforehand.

In addition, you cannot create new categories in the Content Center during the publishing process. Use Content Center Editor to set up the categories beforehand.

When publishing authored parts, map the part parameters to the category parameters. The information you provide to define the part: .

• Sets the structure for its location in Content Center.
• Provides a base for the part file name.
• Makes the part attributes available for future queries.

After you successfully publish custom conduit parts and fittings to the Content Center, you can create new styles based on those published parts.

Most styles require a pipe, elbows, and a coupling. Welded styles do not require a coupling.

Drawing views, parts lists, and the Bill of Materials table specific to the Tube & Pipe add-in describe individual pipe runs and components.

In drawings, tube and pipe information is treated like other parts and subassemblies. You can describe the individual pipe runs and components and detail them using normal drawing manager methods and commands, unless noted otherwise.

The two drawing properties are typically used to roll up conduit parts in the parts lists correctly. You can add them to either specific drawing documents or drawing templates:

• Conduit segment length. With an internal name of Base QTY. It specifies the length of conduit parts.
• Raw material description. With an internal name of Stock Number. It stores the raw material descriptions for conduit parts.

The following guidelines help you create tube and pipe drawings correctly:

• If you are migrating R9 or earlier tube and pipe drawing documents to the current version of Autodesk^® Inventor^®, determine the BOM to use.
• To document individual routes and runs, create design view representations in which you turn off the visibility of unnecessary components. Then apply them to appropriate drawing views.
• Use broken views to fit long nondescript sections of pipe on a drawing.
• Use detail views to show selected fittings.
• To dimension routes and runs correctly, recover route centerlines. To dimension unpopulated routes, you can recover route centerlines.
• Add the Pipe Length and Stock Number properties to parts lists and a Bill of Materials table.
• To create BOMs for specific routes and runs, set their BOM Structure property to Reference.

When documenting a tube and pipe assembly, each new drawing file uses a drawing template. You can update existing templates or create and add new ones into the Templates folder. For Windows^®XP the folder location is Program Files\Autodesk\Inventor<version>\Design Data\Tube & Pipe by default.

A Design View is created in the assembly environment and preserves a designated representation view of assembly components. It can be mapped to drawing views of the assembly file.

If you want to document only specific pipe runs in a complicated assembly, you can define a specific design view. In this design view, components that are contained in the top-level assembly but not within the pipe runs are hidden. Thus, when the relevant design view is selected for the drawing file, components with Visibility turned off do not display.

Before you create drawing views for pipe runs, you can customize specific design views for the assembly environment using the Design View Representations command.

By default, the drawing manager hides the centerlines of tube, pipe, and hose routes in drawing views. Centerline recovery is used to control the availability of the route centerlines in active tube and pipe drawing views for dimensioning.

You can control the centerline recovery at the tube and pipe runs assembly, individual run, or individual route levels in the active drawing view. Base the control on your needs. For example, you can dimension all or most of the routes and runs in a tube and pipe assembly. Include route centerlines for the entire tube and pipe runs assembly, and then hide the centerlines for the individual runs and routes you do not need.

You must dimension routes to the centerlines in drawing views. Otherwise, the dimensions may be incorrect. When the specified route centerlines are recovered, you can dimension routes to the centerlines. If you change the centerline recovery back, all recovered centerlines in the active drawing views are deleted so associated dimensions may disappear or become incorrect.

NoteWhen a new route or run is created, the route centerline in drawing views has the same centerline recovery setting as the parent. To add or remove centerlines for other Autodesk Inventor components in a standard assembly, change the Automated Centerline Settings on the Tools tab Options panel Document Settings Drawing tab.

In drawing views that are created from the base view, the route centerline visibility respects the setting in the base view. For example, if you have recovered route centerlines in the base view, the relevant route centerlines are automatically recovered in all associated drawing views that are subsequently created. When route centerlines are not recovered in the base view, you can manually recover them for drawing views you need.

There are two types of dimensions for documenting the drawing views of the tube and pipe assemblies:

Model dimension

Controls the features that are applied during sketching or creation of the feature. Autodesk Inventor Tube & Pipe can access the model dimensions of components and place them in a drawing view. You can then retrieve them to display the overall dimensions of pipe runs.

Drawing dimension

Added in the drawing view for further documentation using the General Dimension command on the Annotate tab. It does not affect features or parts. You can add general dimensions, baseline dimensions, ordinate dimensions, and so on.

You can use the commands on the Annotate tab, shown in the following image, to add dimensions. Pause the cursor over each image to view the tooltip.

Dimension commands:

• General Dimension
• Baseline Dimension Set
• Baseline Dimension
• Ordinate Dimension Set
• Ordinate Dimension

In a tube and pipe bill of material (BOM), conduit parts and fittings from the Content Center that make up routes and runs are set to Purchased. Master runs assembly, rigid route sketches, hose splines, and hose assemblies are not distinct line items in the bill of materials, so they are set to Phantom.

You can override the default BOM structure to meet your design needs. For instance, if you want to create and export the BOM information for specific routes and runs, set all other routes or runs to the Reference BOM structure. In addition, using the BOM Editor, you can:

• Edit materials.
• Add custom iProperties.
• Enable structured and parts-only BOMs and set view properties accordingly.
• Enable the part number merging and set the merging criteria.
• Set quantity overrides for components.
• Control whether different components with the same part number can be merged into one row. If the merging is enabled, you can create your own list of values to exclude from being merged into one row. The blank part number is permanently excluded so different components with the blank part number do not merge.
  NoteIf you are migrating tube and pipe drawings from R9 or earlier versions, ensure the stock number (Stock Number) and conduit segment length (Base QTY) properties are selected into the BOM table.

If Base QTY and Stock Number properties are not selected into the parts lists, parts lists do not include those properties the first time you create them.

Keep in mind that the drawing manager always groups parts using the Part Number property even if you remove it from the parts list. Each conduit part in the current version of Autodesk Inventor has a unique part number:

You may want to use information that is defined in tube and pipe styles to annotate tube and pipe drawings. You can start to define sketched symbols, and then use the Text command (highlighted below) on the Sketch tab to insert property references in text. When property values change, text that contains the property updates with the new values. Pause the cursor over the images to view the tooltip.

Drawing Sketch panel bar