11/29/2006 - 10:00 am - 11:30 am Room:Delfino - 4003 (PTD Campus)

Getting the Most from Autodesk Inventor® Templates Christiaan Bowen - Sellier Enterprises, Inc.

MA22-2 Struggling with your current dysfunctional drawing templates in Inventor? Are you wondering whether you’re getting the most out of Inventor’s drawing capabilities? Have you ever seen a drawing or part and wonder how to get your template to work like the other guy’s? We will look at how we can use Styles and Standards to best advantage. This course delves into the practical uses of Inventor’s drawing managers and wizards.

About the Speaker: Christiaan is an accomplished instructor and an Autodesk Inventor Certified Expert with over 17 years of experience as a specialist in mechanical design primarily using Autodesk products. Celebrating his 5th year teaching at AU, he combines his expertise, knowledge, and patience to teach innovative courses in the Autodesk Inventor Professional Series products. Christiaan has also incorporated a company, Sellier Enterprises, Inc., that specializes in customized Inventor instruction and mechanical design for industrial automated machines, including high-speed. machine-automated mail sorting equipment. [email protected]

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Getting the Most from Autodesk Inventor® Templates

Templates, why do they command such attention? The reason why it’s important to have a complete template library is time savings which is money saved and when designs are delivered on time and under budget the customer is satisfied. Templates can be set per job or per customer. They can also be set to be material specific. All files in Inventor start with a template which means an attention to detail should be given to the setup of Inventor templates. There are many different approaches that can be taken when template libraries are created. This class will explore practical methods on setting up functional templates in Inventor. Any file type in Inventor can be used as a template as long as the file resides in the templates directory. We will take a look at starting from scratch as well as harvesting styles and standards from other drawings. We will also look at procedures to incorporate templates after a design has been started.

TIP: Then engineer’s notebook can be used to specify instructions on how to specific templates. A quick review the basics, where are templates stored?

Take Note: This handout should serve as a handy reference guide for creating templates and template schemes.

By default, the templates are stored in Inventor’s root directory: C:\Program Files\Autodesk\Inventor 11\Templates. This can reside anywhere you choose by specifying the location through the Application Options dialog under the File Tab. Additional subdirectories can be added to the Templates directory. These sub-directories show up as tabs in the Open dialog box. In order for the tabs to be active, at least one Inventor file is required to live there.

Template Variation The following are examples of template types, recommendations and guidelines to get started.

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Getting the Most from Autodesk Inventor® Templates

Default Templates (.idw) •

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You can set any template to be the default template for creating new assemblies and parts. To make a template the default, save it in the Templates folder with the file name standard.iam. To avoid overwriting the existing default template move or rename the existing standard template before saving the new template. Files that reside in the Templates folder appear on the Default tab of the New dialog box when you create new files. Files that reside in a subfolder of the Templates folder appear other tabs in the New dialog box. These templates are included with Inventor out of the box Template can be used for data translation into Inventor i.e. step or iges. Since Inventor uses the default template to translate data, why not tweak it to suit your needs.

Note: To add tabs to the New dialog box, create new subfolders in the Templates folder and add template files to them. The New dialog displays a tab for each subfolder in the Templates folder. Drawing Templates (.idw) • • •

You can create a template from a drawing, preserving annotations on drawing sheets, such as custom symbols, notes, and revision tables. In addition, your borders, title blocks and view definitions can be retained in the template.. Boarders can be copied from one drawing to the next in the browser. View annotations and general notes are not saved in a template. A possible solution is to create .idw’s containing all notes required for design projects. Variations of Part Templates (.ipt)

The planning starts with the deciding what to include in a part template • • • • • • • • •

For example, any settings that will streamline the creation of parts or establish default values can be included in a template. Small medium and large part templates would be variations of part templates. Changing the grid settings and the size of the origin work planes so that they are more proportional to the part size at the time of it’s creation would be another example. Create a default sketch that has default work features, such as a work axis at the intersection of the three base work planes. Create a sketch on a plane other than XY to change the definition of the isometric view. Add sketches or solid geometry as the start for commonly created parts. If you use different units of measurement in different parts, create different templates for each. Define commonly used parameters or link to a spreadsheet of parameters. Set and define the default material. If you use lighting and color styles, set the styles so that they are available when you want them.

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Getting the Most from Autodesk Inventor® Templates

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Setting iProperties in the Part You can specify properties such as cost center, project name, or manager and save them as part of the template. Properties can be used to find, track, and manage your files. They can also be used to automatically add and maintain information in title blocks, parts lists, and bill of materials. BOM structure can be set for the type of part i.e. Normal, Phantom, Purchased or Reference. This is important because it will drastically affect the outcome of your BOM and drawing. This can be accomplished through document settings.

Importing DWG Data Template For the greatest efficiency when translating data, develop separate templates for opening DWG files. • • • • •

Remove any unwanted content from the templates. This may include sketch geometry, features, or standard drawing views. Set the measurement units and other document settings. Set file properties that are common to the files you import. In part and assembly templates, set up color, texture, lighting, and material styles. In drawing templates, set up drawing resources, dimension styles, text styles, and drafting standards. Variations Assembly Templates (.iam)

Deciding what to include in an assembly template is the hardest challenge to creating assembly templates. Elements to include in the Assembly template: • • • • • • •

Any settings that streamline the creation of assemblies or established default values can be included in a template. For example, changing the sizes of the origin work planes to better accommodate the average size of the assemblies you create. If you use differing units of measurement in different assemblies, create different templates for each. If you use lighting and color styles, set the styles so that they are available when you want them. Associate the template file with a style library, or if you do not use style libraries, define the styles in the template file. Define the columns and format for the bill of materials. You can specify properties such as cost center, project name, or manager and save them as part of the template. Use Properties to find, track, and manage files. They can also be used to automatically add and maintain information in title blocks, parts lists, and bill of materials. BOM structure can be set for the type of part i.e. Normal, Phantom, Purchased, Inseparable or Reference. This is important because it will drastically affect the outcome of your BOM and drawing. This can be accomplished through document settings. Sheet Metal Templates

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Sheet metal style and material type to be set 4

Getting the Most from Autodesk Inventor® Templates

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Partially formed sheet metal shapes can be pre-modeled BOM structure can be set for the type of part i.e. Normal, Phantom, Purchased, Inseparable or Reference. This is important because it will drastically affect the outcome of your BOM and drawing. This can be accomplished through document settings.

• Weldment Template • • •

Set the standard to use. Specify the weld bead material type, visibility, and enabled status. BOM structure can be set for the type of part i.e. Normal, Phantom, Purchased, Inseparable or Reference. This is important because it will drastically affect the outcome of your BOM and drawing. This can be accomplished through document settings.

• Setting the default template The Bolted Connection Template • Each new bolted connection can be created from a template. When you open Bolted Connection Generator, click Set to apply the template to currently designed bolted connection. • Any new bolted connection can be used as a template when you save it to the Templates Library on hard drive. The next time you create a new bolted connection, the new template is available.

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In the upper right corner of the dialog, there are two tools to note.

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Getting the Most from Autodesk Inventor® Templates

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Settings – This sets where the bolted connection will live

Enabling/Disabling Calculation – If you don’t require this feature for you design process, turn it off.

Templates Library is displayed when you click the More Options button in the right lower corner of the Design Tab. Each new bolted connection can be created from template. When you open Bolted Connection Generator, click Set to apply the template to currently designed bolted connection. Any new bolted connection can be used as a template when you save it to the Templates Library on hard drive. The next time you create a new bolted connection, the new template is available. •

Set – Applies the characteristics of selected template to current bolted connection

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Add – Use a new template to add designed bolted connection to the template library. Add button is available only when complete geometry of bolted connection is specified i.e. start plane, reference and an end plane.

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Delete – This option deletes selected bolted connection template.

Editors and Wizards to Guide you through the template creation process They can be found here:

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Getting the Most from Autodesk Inventor® Templates

Drawing Resource Transfer Wizard • •

Use the Drawing Resource Transfer Wizard to copy drawing resources such as borders, title blocks, and sketched symbols from a source drawing to one or more target drawings. You must close Autodesk Inventor before you can use the wizard. Harvesting resources from the drawing resource transfer wizard will be explored. In order to access the wizard, Inventor must be closed. This is a great tool to pick and choose what needed to design the ultimate template. Use the Drawing Resource Transfer Wizard to copy drawing resources such as borders, title blocks, and sketched symbols from a source drawing to one or more target drawings. You must close Autodesk Inventor before you can use the wizard.

Here’s how it works: First – Select the Source drawing from where the information will be pulled from.

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Getting the Most from Autodesk Inventor® Templates

Second – Select the target files of where the drawing data is to be sent. Notice you can select multiple files.

Third –Inventor now prompts for an option and sends a warning. Option – The Drawing Resource Transfer Wizard can replace resources in the target file(s) with resources of the same name in the source file. Warning – If you replace resources that contain prompted text, some data loss is possible if the source and target resource prompted fields do not match. In other words if Yes is selected that information could get overwritten. Fourth –Select Start and let the Batch Processing Begin! Inventor will now kick out a report which can be copied and pasted into a text file for future reference.

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Getting the Most from Autodesk Inventor® Templates

Styles Management Wizard This wizard will assist you in simple batch style management for your Autodesk Inventor files. The following batch processes can be performed:

Harvest Styles This batch process can be used to take any styles from your Autodesk Inventor files and place them into a target Style Library. This is a tremendous aid when trying to reuse information into a template structure. Purge Styles This batch process is used to remove any unused style information from your Autodesk Inventor files. This is beneficial for large assemblies because it can reduce the memory footprint, leading to a potential increase in capacity for your large assemblies. • • • •

The Style Management Wizard is a tool for administrators to assist in batch-style management for Autodesk Inventor files. Using the Style Management Wizard, you can: Harvest styles from Autodesk Inventor files and place them in a target style library. Purge styles from Autodesk Inventor files. Purging removes unused style information and can be beneficial in very large assemblies by reducing required memory. Use the Style Management Wizard when transitioning to using a style library with your design project.

Here’s how it works: First – Lists all defined projects by Name and Project Location, the active project is indicated by a check mark. Its settings for Style Library and path are summarized below the window. Doubleclick to select a project and make it active. The Style Management Wizard uses the active project to resolve all file paths during processing.

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Getting the Most from Autodesk Inventor® Templates

Second – Select the files to Process. Selects files to process in a detailed view.

Add Specific Files button – Browses to the folder that contains the files to process. Selected files are listed by file name, file type, and path.

Add All Files in Active Project button – Lists all files by file name, type, and path. Clear the check box to exclude a file from processing. Alternate methods of adding files to the list: Drag and drop files from Microsoft Windows Explorer. Drop them in the list to add them. Get all files referenced by a specific file by right-clicking the file in the process list, and then selecting Get Referenced Files. Adds all files that the selected file is dependent on to the list. Get all drawings or presentations that use a specific file by right-clicking a file in the process list. Select Drawings and Presentations, and then Get All. Adds to the process list all drawings and presentations in the project.

Third – Select files to manage Chooses a harvest or purge operation. Harvest Styles into Target Style Library specifies the target style library. Use Source Project Style Library Automatically selects the style library specified in the project. Clear the check box of files you want to exclude from processing.

Create a New Style Library - Opens the New Style Library dialog box. Specify to copy an existing style library or create an empty library, browse to the folder where the library will be stored, and if copying, the source style library you are copying.

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Getting the Most from Autodesk Inventor® Templates

Select an Existing Style Library – Lists the Default Style Library and any project that uses a style library. Use the Browse button to browse to a specific library. Purge All Unused Styles from Files – automatically deletes unused styles from selected documents. Styles not saved to a styles library are permanently lost.

Fourth – Start batch processing operation.

The harvesting now is complete.

Styles and Standards Editor This editor is for the styles editing of assemblies, parts, drawings, and presentations

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Getting the Most from Autodesk Inventor® Templates

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Creates and edits styles. Styles defined in the Style Library and in the active document are listed in the browser pane; available styles depend on the current document type. The selected style contents are shown in the editor pane.

For the current document, you can click: • • • • • • • • • •

Back to return to the previously edited style. You are prompted to save the previous edits. New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style. Save to save changes to an existing style in the current document. Reset to return style values to the saved values. Filter to show Local Styles, Styles in the Active Standard (drawings only), or All Styles in the browser. Import to use the Import Style Definition dialog box to import a style exported from another document. Name Identifies the selected style. Location Indicates if the style is located in the Style Library, the current document, or both. In Use Indicates if the style is being used by the document. Changes Indicates if changes have been made to the style. If changes are made only in the current document, the entry is labeled Local. If changes have been made to the Style Library, the entry is Library. If both the local and library styles have been changed and the values do not match, the entry is Both.

Styles Library Manager This tool can be used for comparing and copying styles between Inventor files.

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Getting the Most from Autodesk Inventor® Templates

Management of the dialog box - When copying a style library, if a source style and one or more of its substyles differ from the destination library, you are asked to select which substyles to copy to the destination library. For example, a dimension style uses the text style as a substyle. If the text substyle referenced by the dimension style is different from the text style in the destination style library, you must confirm to replace the destination text style with the text substyle from the source style library. If you choose to use a combination of Yes and No in the Overwrite column, the style in the destination style library will not have identical characteristics compared to the source. • • • •

The Style Library Manager is used primarily by a CAD administrator to: Copy styles from one style library to another style library. Rename styles in a style library. Delete styles from a style library.

Any changes made to a style library are not available in other documents until the current Autodesk Inventor session closes and a new session is reopened. Some styles reference other styles as substyles (for example, the dimension style references the text style as a substyle). When copying a style library, the Style Library Manager opens the Manage Styles dialog box if mismatched substyles are detected in the source and destination libraries. For each substyle you must confirm to replace the current version with the source version.

Here’s how it works: First –Choose Style Type – This selection lists all style types. Click a style type to show all definitions in the Style Library column. Second – Click Style Library 1 to browse to the appropriate style library. Third – Click Style Library2 to Creates a new style library by copying an existing library or creating an empty library, specifies its location, and names the source library to copy, if applicable. Fourth – Select the appropriate filter button

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Getting the Most from Autodesk Inventor® Templates

Click Show All Styles to list all styles in both style libraries. Click Show Mismatched Styles to show styles whose definitions are different in the two libraries. Click Show Unique Styles to show styles that exist in one library but not the other. >>Copies selected styles from Style Library 1 to Style Library 2.