Solving Inventor Template Style Conflicts

I have been seen many Inventor users encounter the following error every time they create a new Inventor file and simply live with it by selecting OK and moving on.

It normally is more a nuisance instead of a problem but why accept it when the solution is relativily simple.  The first thing to understand how Inventor templates and Design Data are related.  By the way, Design Data is often called the Styles Library so do not confuse them, they are identical.  Inventor templates contain certain configurations for example text styles, dimensional styles, layer settings, etc.  There are a vast number of configuration settings, especially in the 2D drawing template but I will just use text styles for this article.  Inventor Design Data also contains configuration settings for all Inventor template types.  Both of these and their location are declared in the Application Options or in the current Inventor Project file.  I am a fan of using the Inventor Project file to declare the current template and Design Data files and their location.  I have two reasons for this, one I do not want to modify the default Inventor templates or Design Data because I want to always have a clean source if I want to build a new configuration.  Sure I could backup the originals before modifying them but you know how that goes.  The second and main reason is that I can declare a different set of templates and Design Data for different project files.  This does not mean I use a different project files for each company project, I only use one project file for all company work.  Many companies often have to design work for other companies using their templates and Design Data.  If this is the case I can have a project file for each company and each project file declares the templates and Design Data for their work.

Getting back to the reason for the "Style Conflict" error.  If the Inventor template configuration does not match the Design Data configuration, you will get this error.  I will not go into the reasons it happens, I just want to tell you how to solve it.  First of all one person in the company should be in charge of Inventor templates and Design Data.  This person should create a special Inventor project file dedicated to template and Design Data creation.  This project file declares three main things, that the Style Library (Design Data) is Read-Write and the location of the Design Data and and the matching templates.  Note the screen shot of my Inventor 2018 Template Work.ipj file and the marked areas.  If you use the Vault, this project file should be a Single User type.  The red arrow is simply trying to explain that the ".\" entry for Templates location is the same as the location of the project file itself.  Make this project file active.

The next step is to open up the offending template and select the "Update" icon under the Manage tab, Styles and Standards panel. 

You will see the style that is conflicting.  In my example it is only one but there may be many more.  At this point STOP and ask yourself, "Is the Design Data configuration correct or is the template?"  If it is the template, select "Cancel" and read on later in this article.  If the template needs to be updated to match the Design Data (Styles Library) then select "Yes to All" icon near the bottom of the dialog box and then select "OK" to finish.

Inventor will give you the following message which basically says you are updating the template to match the Design Data, the cause of the error.  Select "OK" to continue.

Next, save the template and close it.  Since this is the only template I am editing I will return to the standard company Inventor project file and test my work.  If you have more than one problem template, repeat the steps for each template before switching project files.  

When you open the template file, the error message will not appear.  Congratulations, you have fix your company template file(s).

So now we want to think about what to do if you earlier decided that the template file is correct and the Design Data should be updated to match.  Instead of selecting the "Update" command, you will select the "Save" command right above it.  This will save the template configuration to the Design Data folder.

 

 

Do not forget to choose "Yes to All" before selecting "OK" to be sure you are actually writing the changes to the Design Data.  Since you have written new data to the Design Data folder, all other templates may be out of date and do not match the new Design Data. The original error will appear for them as well when they are opened.  After writing new configurations to the Design Data folder, you must open each Inventor template and follow the "Update" procedure for each outline above.  Remember all of this must be done while using the Inventor project file you earlier created for editing your templates and Design Data.

 

This may sound like a lot of work but it actually only takes a couple of minutes.  The configuration of the original templates and Design Data to match your company standards is the real work and may take you many hours.  By the way when you upgrade your Inventor version all templates and Design Data must be migrated.  The process is similar once you have migrated the Design Data using the installed Inventor Styles Manager.  That could be a new article I will try and tackle later.

 



How to Include a Dynamic Part Number in the Part Drawing View Label

There are various methods of detailing machine parts in Inventor.  Some companies use the method of one part per drawing while others desire to place multiple part details on one drawing.  A common practice is to place part detail drawings as sheets under the top level assembly drawing.  When the decision to place multiple part details on one drawing is used, Inventor needs to be configured to place a unique view label for each part to avoid confusion by fabrication personnel.  This view label must also be dynamic so if the part being detailed is changed, the view label will update to reflect the new part information.  Below is an example of this type of drawing showing view labels containing the part number of each placed part.  The configuration of Inventor to place a dynamic view label, containing the part number, is the focus of this article.

The process beginnings with the editing of the drawing template and the controlling Design Data, sometimes referred to as the Styles Library.  This article will not go over the process of creating a set of Inventor templates and their matching Design Data but it will cover the drawing style configuration, contained in the template, to accomplish our goal.  A drawing template is configured to follow a defined Active Standard as shown in the Document Settings dialog below.  If you open one of your Inventor drawings and choose Document Settings on the Tools tab under the Options panel, you will see the this active standard.  It is coming from the Design Data folder which is defined either in the Inventor Project File or in the Applications Options.

For demonstration, I will be modifying the Design Data for a single demo drawing which will not be permanent for all future drawings.  To make it a permanent setting, the Design Data library must be edited.  For this one drawing I select the Styles Editor command which can be found under the Manage tab on the Styles and Standards panel.

In the Styles and Editor dialog box, I select my Standard then the View Preferences tab.  Notice that the editor is in Read Only mode since I am only editing this one drawing.  

The View Label Defaults is the area where I can configure the information that will be included in my base view label.  The first thing I will set is which model property will be displayed in the view label.  In the Display panel you will notice the standard Inventor view label configuration.  Selecting the "pencil" icon will display the following dialog box.  Follow the numbered steps to replace the default <VIEW> entry with the model property "Part Number".  Select "OK" to finish.

Next I will leave the View Type on "Base" since I want the view label to be automatically placed  on the base view of each part.  Last I will choose the position of the view label and select the Visibility icon to make the bulb "light" indicating that the view label will be displayed.  I finish by selecting Save to exit the Styles Editor.

When I place the base view of my part along with any projected views and select OK the view label appears under the base view.  At this point you can drag the view label to a different position if desired.  If the base view is moved, the label will follow it.

If I wanted to add "PART NUMBER" to the label entry, I simply add it as text in the Display dialog box.

To prove this part number is dynamic, I will use the "Replace Model Reference" command to replace the part in the drawing view.  This command is located on the Modify panel under the Manage Tab while in the drawing.

As you can see, if this modification was made to the Design Data library for all drawings it will make the management of multiple part drawings a lot easier.

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!