Creating a Material Cut List for Your Inventor Drawings

In this article I will be developing a Material Cut List to automatically report cut lengths for common materials used in Inventor.  I will be developing this for one drawing and will not go into the process of editing the project design data and templates to make it available for all drawings.  The process is the same for the most part, only the method of saving the design data will not be covered.  I will be using an Inventor IDW drawing format but the process is identical if your company uses the Inventor DWG drawing format.

Normally cut sizes are applicable to four Inventor standard components.  These are:

• Sheet Metal Flat Sheet Extents
• Content Center Standard Structural Shapes such as angles, channel, and tubing
• Hose lengths either from a routing assembly or lengths used directly in a design
• Pipe and Tubing lengths also from a routing assembly or lengths used directly in a design

Below is my example drawing with one of each standard component.  I have use both a pipe and tube section just to illustrate.  The Material Cut List is the same for both so if you configure for one you will be set for the other automatically.

Keep in mind that the format of the cut lengths and the column headers are fully configurable, you are not restricted to my selections.

The first place to start is to configure your Inventor part template to capture three properties of sheet metal parts, the Sheet Metal Rule which will report to the stock number column, the sheet metal flat pattern width and length.  These configurations are added to your sheet metal template as custom properties.  These custom properties are set to report standard sheet metal properties.  Below I show the custom properties with my chosen names, yours can be anything you desire.  Please note each one is has a function for its value.  SML stands for the sheet metal flat length, SMW the sheet metal flat width and the Sheet Metal Style will report the name of my sheet metal rule which is my material description.  

After selecting an iProperty the value function can be edited using the icon marked with the red arrow.  The initial entry is typed directly into the value box.  The three iProperties and their value functions are:  (the equal sign is a part of the value function.)

• SML  =<Sheet Metal Length>
• SMW =<Sheet Metal Width>
• Sheet Metal Style =<Sheet Metal Rule>

Enter and save these in your Inventor sheet metal template and you are all set.  The Inventor custom iProperty value for structural sections, pipe, hose and tubing are entered automatically during component placement so no modification to your part template is required.  The custom iProperty name for each is listed below.

• Structural Sections - G_L
• Pipe, hose and tubing - PL

The next configuration to to develop a Material Cut List in your Inventor drawing template.  Open up your drawing template and select "Styles Editor" under the Manage tab in the Styles and Standards panel.

Make sure that your are editing your company Design Data standard, expand the "Parts List" entry and right click to on the title to create a new parts list style called Material Cut List.  

Next fill in the title, select the desired text styles and choose other appearance settings to suit your company standards.  The main configuration is to select "Column Chooser" which will allow you to choose what Inventor iProperties to report in the Material Cut List.  

Some of the iProperties are listed in the "Available Properties" table but all custom iProperties are not and you must enter them using the "New Property" icon.  Remember to add the exact custom iProperty name, not what you want the Material Cut List column will eventually read, this is added later.  For example, one of my custom iProperties is PL so this is what I enter in the Define New Property dialog box.

Continue until you  have all the iProperities added then select "OK" to return to the configuration table editor.  You will notice all the selected and entered iProperties are shown in the list.

The next step is to click on each column header and edit the name to whatever value you would like to appear in the finished placed Material Cut List on the drawing.  Keep in mind that names will word wrap if they exceed the column width which is entered in the next column.  You may have to practice with column widths to decide which is best for you.  You can always resize the list after is is placed on the drawing but it is not desirable. 

The next step is to right click on each Property and select "Format Column".  I will start with the Stock Number Property.

The only change I need here is for the Stock Number to report the custom iProperty Sheet Metal Style if it exists.  This is accomplished on the Substitution tab as shown below.

The G_L property has two changes, one to configure the column units format and the value column justification.

The second in to enable value substitution if the component is not a structural component but a pipe, tube or hose.  We would like the PL iPropety value to replace the G_L value if this is the case.  Also you will need to configure the units formatting to use if the substitution occurs.

You will need to configure the last two properties using the Column Format tab to set units display and data justification following the same process used earlier.  When finish, select "Save and Close" to save the changes to the drawing template.  I want again to remind you that I am only configuring the Material Cut List in this drawing, if you are configuring for all drawings, these configuration settings must be exported to the company Inventor design data and template files.

Once you have your drawing view created, you now want to place the Material Cut List.  The placement is accomplished by selecting  "Parts List" command under the Annotate tab and then selecting Material Cut List from the Format drop down.  The process from this point is the same as if you were placing a parts list in the drawing.

One last note, if you have configured your Material Cut List to report sheet metal flat pattern extents you must have developed a flat pattern to have the values populate.  Enjoy!

Importing Inventor Sheet Metal Styles

You may be building a new Inventor Sheet Metal template and want to populated it with sheet metal styles from another template.  Often sheet metal styles contain extensive bending data, notching configuration and other sheet metal settings and it is impractical to recreate sheet metal styles just because you are creating a new template.  You may have acquired a customer's sheet metal styles and wish to incorporate them into your templates for a special job.  No matter the reason you would like the most efficient method of copying them into your production Inventor template.

The first thing I recommend is to develop an Inventor project file that is dedicated to template work.  This project file will be a single user project even if you company is using the Vault.  The only purpose of the project file is to edit your Inventor templates and design data.  This project file is normally located in your template file folder but this is only for convenience.  Under the folder options point the Design Data to your production design data folder and your Templates to the folder containing your templates.  In my case, my project file is located in the templates folder so it is denoted by a ".\ "  The Content Center Files path is not important for this project file but can be set if desired.  The last thing that needs to be set is the "Use Style Library" which should be set to "Read-Write" to allow the addition of any new or updated sheet metal styles to the Design Data folder.

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There are two basic ways to copy sheet metal styles.  You can copy one at a time from one template to another or use the Inventor Style Library Manager to copy, or remove, as many styles at one time.  I will show the one at a time method first which is valuable when you want to maybe copy one or two sheet metal styles from one template to another.

Open up the sheet metal template you will be copying from.  Select the desired Sheet Metal Rule from the Style and Standard Editor dialog box and right click.  Select "Export" and give the "styxml" file a descriptive name and save it.

Open up the template you would like to copy the style to and select "Import" at the bottom of the Style and Standard Editor dialog box.  Browse to the previously save "styxml" file and open it.  The style is imported and placed in the list.

If you wish to make all the sheet metal styles in the template available to all templates, save them to the Design Data folder.  Open up the template containing the sheet metal styles, select "Save" in the Styles and Standards panel.

 

 

You can select which styles you will be saving or select "Yes to All".  In my example I have only selected the sheet metal styles and de-selected the unfold rules.  Normally the unfold rules will be saved as well but I am not finished their configuration at this time.

 

 

Switching back to your production Inventor project file you will notice that when you open up any sheet metal file, either old or new, the sheet metal styles will be available.  This is because the production Inventor project file is pointing to the updated Design Data folder.

 

You can also use the Inventor Styles Manager to copy files between two Design Data folders.  The Inventor Styles Library Manager application is found in the All Applications listing in Windows 10 or under the Start menu in Windows 7.

 

 

Open up your Design Data folder containing the new sheet metal styles on one side of the application and the Design Data folder you wish to copy to on the other.  The sides you choose is up to you, just keep them straight so you do not make a mistake.

 

 

Using this utility is the best way to delete unwanted Design Data styles as well.  Simply right click on the style(s) you wish to remove and select "Delete Styles".

 

All of the above discussion applies to other Design Data styles such as dimension styles, text styles, part lists, etc.   Getting the right styles in your Inventor templates is a simple and straight forward process.  Creating the original styles is the hard part.  My suggestion is to find an Inventor template with styles you trust and copy it!