Windchill PDMlink

Windchill PDM link Primary objects
1. Documents - all types of computer files *.avi *.txt *.jpg
2. CAD documents - all types of Pro/E or any cad software files
3. Parts and end items -They build product structure, they do not contain cad documents but make a reference
4. links - Hyperlinks to web pages to outside the enterprise
5. Change items - used to store change information of other items. It includes problem reports, change request and change notices.

WT Parts (Windchill technology parts or PDMlink parts)

In general, a WTPart represents a set of metadata (attributes and other related information) that is used to describe a CAD document, such as a Pro/ENGINEER part or assembly. A WTPart does NOT have any content. Instead, it may have a representation of the CAD file, such as a ProductView image. Usually, a WTPart contains more information than what is contained in the CAD document. A WTPart is normally associated with a CAD document, and/or other type of documents such as Microsoft Word or Excel. Therefore, the part can be considered as a center point from which you can navigate to other areas of the assembly, such as a CAD file, a Word document, or other objects.

You may wonder why you need a WTPart, and whether can you just use the CAD document instead. In Windchill, you may choose to represent your assemblies using CAD documents alone, or with WTParts that are described by CAD documents. There are distinct advantages to using WTParts.

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WTParts may be created manually and have no CAD document associated with them. This is useful for purchased parts for which you may not have CAD files, or if you do not have the workgroup manager needed to create a CAD document from the CAD file provided by the supplier.

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WTParts may be associated to different view versions. For example, a product may have two separate BOMs for the same product, one design view and one manufacturing view. If you use WTParts, both view versions of it may be described by a single CAD document but allows for the restructuring of the BOMs. This ensures that both manufacturing and design use the same CAD file.

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Multiple WTParts or versions of a WTPart may be represented by a single CAD document. This may reduce the storage space required by the system.

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You do not need a workgroup manager or CAD application to create WTParts. You may describe your WTParts with documents, or choose not to describe them at all.

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You can also manage occurrences, allocation, and incorporation, and use serialized parts.

For these reasons, it is a best practice to manage CAD information using WTParts and CAD documents. However, some organizations may not require the additional functionality provided by WTParts and choose to solely use CAD documents to represent their CAD information. PDMLink fully supports both approaches.

There are two types of WTParts, the part and the end item. Consider the end item as the salable object. The WTPart/end item structures enable you to perform additional configuration management operations, such as creating end item configurations and end item instances.

There are two types of links that connect the WTPart and CAD document. They are called owner and content links. There can be only one owner link for each WTPart, but there can be any number of content links. Metadata, such as the parameters/attributes and the viewables, are propagated to the WTPart from the CAD document by means of an owner link.

There are also various design approaches, such as CAD-centric, Part-centric, and a combination of the two. In the CAD-centric method, you design CAD models first, and then create (manually or automatically) and associate the WTParts. Contrary to that, the Part-centric method is used when you want to have the product structure (eBOM) in the system; this occurs during the concept phase. The CAD design begins, but is associated later. You may also want to start your marketing campaign for the product, but the CAD design is far from conception, so you create WTParts to provide a record in the database. Moreover, the empty WTPart structure enables you to route it through the workflow process and perform other data management operations. The WTPart structure may or may not be identical to the CAD structure.

Pro/Program

Pro/PROGRAM is a simple programming interface that may be used to create interactive parts. Pro/PROGRAM requires very little programming knowledge (you do have to understand IF statements). It is a simple, dynamic tool for creating variations of a design through a definable user interface.

Pro/PROGRAM can be used to create different configurations of any design that has standard variables that govern the modifications. Whenever you create a part, data is stored in its database that describes how features are created. This data may be edited in a text file by choosing the Program option from the Tools menu. For example:

You can edit this program to add logic that will add or not add features based on IF statement evaluations. You can also add mathematical computations, interactive prompts to get information from the user, etc. Whenever the part or assembly that defines the program regenerates, the program is automatically run.

For example, an elevator button panel has a standard set of variables that govern the different variation of the design: number of floors, two or three columns, whether or not there is a level below the lobby, etc.

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Version 2

Figure 1

You could create a Pro/PROGRAM of a completed panel assembly that prompts the user for these key variables and either modifies dimensions to correct sizes or swaps models in and out of the final assembly depending upon the configuration.

Pro/PROGRAM is like a dynamic family table, where a simple BASIC-like program prompts the user for inputs, then drives the design. The inputs can be numbers, strings, or yes/no parameters, and can drive dimensions directly (What is the length of the box?) or alter geometry through if-then-else loops (Do you want the hole?). The model is displayed as its information structure, with each feature in a block of text. If a loop is placed around the text, this feature can be turned on or off depending upon the requirements.

There are several items of note in this example. The input variables can be yes_no, numbers, or strings. The prompt for the input can be user defined if placed directly below the input line. The inputs can be varied through if-then statements. The variables can be passed to dimensions through relations or to geometry through if-then statements. The user will be requested to run the program every time they regenerate.

Note: If the dimension parameter symbol is set to the same name as the input variable name, no relation is required.

Relations in Pro/Engineer

Relations are a very powerful part of Pro/ENGINEER and should be well understood for several reasons:

1. Relations leverage the parametric capability of the system to allow you to greatly simplify the process of making dimensional changes.

For example, without relations, you may have to Edit several dimensional values to alter a part properly. With relations defined, you allow other users to alter only one dimension or relation value while driving many other dimensions.

Relations also can be created to solve simultaneous equations iteratively.

2. Relations can be used to document and maintain your design intent. Relations tell other users why your design works the way it does; and you can maintain critical design relationships.

For example, the easiest way to tell others that the wall thickness is a function of the diameter is to create a relation that drives the model to behave that way.

3. Logical functions can greatly enhance your design intent.

For example, you can automatically define the quantity of holes or cuts based on the size of the part using IF-THEN-ELSE statements.

4. Assembly Relations minimize the parent/child problems of relating different parts of an assembly to each other.

For example, consider the case of creating matching mounting hole patterns on two different parts of an assembly. Rather than creating Coaxial holes, or Use Edge cuts, on the second part, Unalign all your Use Edge cuts, and create assembly relations to drive the 2nd part's hole dimensions to be the same as the 1st part's hole dimensions.

Important procedures:

Define dimension symbols - This is one of the most important steps to self-documenting relations that make sense. Many users do not properly name dimensions and find out later on that their own design confuses them.

Comment your relations - Since you are documenting your design intent for yourself and others, you want to make sure that the relations file contains detailed descriptions of what each relation accomplishes. Comments are placed in the relations file by starting the line with a slash and an asterisk (/*).

Sort your relations - If your relations are not in a logical order, you will be prompted to Regenerate multiple times.

Know that by default, relations are computed before the part features are regenerated. Pro/ENGINEER will first look at the current values of all your feature dimensions, then plug them into the Part relations and get the resulting values; then the features are regenerated based on those results. If a Section or Feature relation drives one of those original dimensions to a different value, you will be prompted to Regenerate Again (possibly an infinite loop of regenerations).

You must also know that there are distinct differences between Part, Assembly, Section, and Feature relations.

Part relations rely only upon the regeneration of a single part to take effect.

Assembly relations rely upon the regeneration of many parts and/or subassemblies. A good use would be for as assembled part sizes: Springs, Shims, Seals. They are also good for matching mounting holes and features between different parts.

Assembly relations are also dependent upon the completeness of the assembly to succeed. For example, an assembly relation relies upon the component number of a part to be valid (e.g. d22:6). If the component with that number is removed from the assembly, the relation will fail leaving your existing part's dimension unchanged but manually modifiable.

When relations are used in an assembly, Assembly relations are computed before the assembly is regenerated and before the part relations are computed. This means that Assembly relations, assembly features, and mating conditions are resolved before part relations are computed. Some complex assemblies may require two regenerations to fully update.

Section relations are used to relate and drive the dimensions of sketched elements within a single 2D sketch, such as a variable section sweep. These relations only affect section dimensions and get evaluated at the time of the feature's regeneration.

Feature relations are very similar to Section relations except they can also drive the 3D dimension values, such as the Depth of a cut. These also get evaluated at the time of the feature's regeneration.

The Analysis Datum is a feature that gets evaluated at its place in time according to feature order. It can then be used in a Feature relation by referring to the Analysis Datum's Feature ID or fid.

There are two ways to specify which editor you want to use when writing relations. Both are controlled by config.pro options. If new_relations_ui is set to no, then the option relation_file_editor controls which editor to use. This option can be set to protab or editor. The protab option causes the Pro/TABLE editor to be used, and the editor option causes the default system editor to be used.

If new_relations_ui is set to yes, the relations editor shown below is used. In this case, it does not matter what the relation_file_editor option is set to, The system ignores it.

Figure 1

Pro/Engineer layer functionality.

This is about Pro/Engineer layer functionality.

We can control the display of non-solid features in Pro/E using layers

Following most important things about layers.

Hide/unhide layer- The Layer / Hide option allows you to remove objects from the display based upon the Layer they are assigned. When you Hide a Layer, its icon is darkened (in the Layer Tree).

Activate layer - When you choose Layer / Activate, all eligible objects created from that point forward (in your part) are automatically members of that layer. Eligible objects are feature dimensions and any drawing objects (e.g., 3D annotation objects). This allows you to automatically aid in the creation and management of drawings made from your part (or of an assembly containing the part when the assembly is placed on a drawing).

Isolate layers - The Isolate option allows you to quickly display the contents of one Layer while removing the contents of all other Layers from the screen. When a Layer has been Isolated, the system displays a different icon next to its name in the Layer Tree.

Suppress by layer - You can select features by layer for suppress operation. You can remove features from the topology of the part using the Suppress option. Suppressing is similar to Deleting features except that Suppressed features are not permanantly removed from the model and can be Resumed later on. However, Suppressing a feature raises the same concerns as Deleting one in that if it is a Parent to other features, they will fail to Regenerate.