Styles Conflict – Inventor Drawings

Posted on September 15, 2015 by Synergis Manufacturing Product Support Specialist, Mark Lancaster

Have you ever seen this message when you start an Inventor drawing?Mark1

Does this message only appear for certain users? Well today I want to share why this is occurring and how to resolve it.

When Inventor is first installed, standard drawing styles are stored by default in the C:\Users\Public\Documents\Autodesk\Inventor <version>\Design Data folder. In the folder there are numerous XML files that are related to the styles listed in your drawing styles editor. These styles/XML files are considered to be they “Style Library” definitions or global styles.

For example:


When you create (or edit) your template and modify the already provided styles (through the drawing styles editor), you are only modifying them within your template and the actual style definition located in the design data folder is never updated.  For example, if I modify the provided Balloon (ANSI) style in my template, the modification is only occurring at that level.Mark3

Now when you start a drawing using your template, Inventor compares the “Style Library” definitions with the ones that you have in your template/drawing.  If they’re different, the styles conflict message is issued to indicate that.  If you look closely at the message, there are a couple of things it is telling us.Mark4

This highlighted portion is indicating the following styles located in the template are different than the ones in the “Style Library” definitions.  If I select the OK button, my styles will be overwritten by the ones that are defined in the “Style Library” definition.  Meaning the style modifications you made in your template no longer exist for this new drawing.  However, many users get confused when they go back to edit their template and find their modifications are still there.  So they ask why my styles are not appearing in the drawing I just started…

The key to this style conflict is based on the comparison that Inventor performs when a drawing is first started using the Inventor NEW command.  When you directly open your template (or an existing drawing) there’s no comparison being performed between the styles located in your drawing and the ones stored in the design data folder.

So now that you understand why the message is appearing, let’s start discussing how to resolve it.  First of all, Inventor is always assuming the “Style Library” definitions located in the design data folder is the controlling factor (styles) for your drawing.Mark5

For this highlighted portion of the message, Inventor is informing us how to resolve the style conflict.  For the former, if the actual “Styles Library” definitions are supposed to be used, then we need to update the styles in our template.  To update, simply open your template, select the Manage ribbon tab and the Update styles function.Mark6

For my template you can see the 4 styles that are listed here, are the same ones that appeared in the style conflict message I received.  When you update, you’re basically overwriting the selected styles (Update column = Yes) with the information residing in your design data folder.  Once the update is performed, the styles now match and the conflict no longer exists.  However, when using this workflow you will lose any modification you made to these styles and in certain cases you probably don’t want this to occur.  So ask yourself do I really want to update my styles or do something else?

For the latter solution, it tells us to use the styles manager and remove them from the “Styles Library” definitions.  So the first question you’re asking yourself, where is the Styles Manager located?  This utility is located outside of Inventor under the Windows start menu/Autodesk/Inventor/Tools section. Mark7

The Style Library Manager performs two functions, one as a migration tool to move styles from one Inventor version to the next and the second is to control you current styles and resolve the conflict message.  However, before using this utility I strongly suggest that you backup your design data folder just in case you make a mistake and want to restore your original out of the box information.

The first thing you need to do is check to make sure the Style Library 1 field is pointing to the correct location where your design data folder resides.  Now select the “Show All Styles” button.  Next select the style type from the list.  For my example I am selecting the Balloon style type.  For the final step, right mouse click on the style causing the conflict and select Delete Style.  In my case it will be the Balloon (ANSI) style.Mark8

However, this is the reason why I’m not a big fan of this method.  The Balloon (ANSI) style has a relationship with other styles within your design data folder.Mark9

Meaning I would have to remove it first from the other styles that are listed in the resulting window.  Is this something you (or I) want to do?  If you want to continue, locate the styles in the order they’re listed and perform the delete style step as I mentioned earlier.  In my case I don’t really want to do this because I truly don’t want to destroy all these relationships that were already formed.  So the question remains, how do I resolve this?  Although the style conflict message doesn’t allude to it, there are 3 other options you can use to resolve the conflict.

Option 1:

By using your template, you can save the styles back to the design data folder and define what the new “Style Library” definitions will be.Mark10

For a certain amount of Inventor users, the “SAVE” option may be disabled/greyed out just as the image above shows.  The reason is based on the setting within your active project file.Mark11

When the “Use Style Library” option is set to read-only, the user is unable to save back to the design data folder.  It’s just another security measure put in place to protect your controlling styles.  When it’s set to read-write then the user is able to save back to the design data folder and update the controlling styles.  So if you’re planning on using this option to resolve the conflict, I strongly suggest that you back-up the design data folder just in case you make a mistake and want to restore your original out of the box information.  In addition I would recommend that all users not have the ability to read-write to the styles library located in you design data folder.

Option 2:

This option, which is my preferred method, is to create new styles in your template from the existing ones and leave the out of box ones as is.  This way when the style comparison is performed, these styles only appear in the drawing template and there is never a conflict.  Stay tuned for my next article that covers how to configure your styles using this method.

Option 3:

With this option you will create a new design data folder location that will contain blank XML files related to the out of box styles.  When the comparison takes place, there are no styles to compare it to, thus no conflicts will ever exist.  The first thing you need to do is to create a (blank) folder location where the new design data will exist.  For my example I created a folder called “New Design Data” on my “D” partition.  Next launch the Styles Library Manager and select “Create New Styles Library”.Mark12

From there change the creation method to “Create Empty Style Library”Mark13

Follow by browsing to the location where you specified your new design data location.  In my example the location is D:\New Design DataMark14

Select OK and Inventor will now create a new design data infrastructure at that specified location.  Next you will need to return to Inventor and define the new design data location either using Application Options or your active project file.

The last thing in resolving the styles conflict is to make sure everyone in your organization is using and/or pointing to the same design data information.  If everybody is using different information, the users will continue to see this message.

Yes, the “Styles Conflict” message can be frustrating at times while trying to resolve it.  Hopefully the information I provided today will help you understand why it occurs and how to resolve it.  In addition please stay tuned for my next article in how to create your own styles and avoid the conflict completely.

Until next time…

Mark Lancaster joined us back in August 2013. His most previous experience is as the CAD Design Manager of Pall Corporation, one of our long time customers. In that position, he was responsible for workstation optimization and design management, established uniform standards for the local and global offices, and developed global systems to control and manage their design data.



  • I’ve read all of the above & my Inventor 2017 behaves as described, this said I’m interested in option 2, as stantard line thicknesses & colours are not what I require also some of the dimension setting i’d like to alter.

    Option 2:

    This option, which is my preferred method, is to create new styles in your template from the existing ones and leave the out of box ones as is. This way when the style comparison is performed, these styles only appear in the drawing template and there is never a conflict. Stay tuned for my next article that covers how to configure your styles using this method.


    • Access the active Inventor project and make sure it’s not set to read-only. In my example the active project is set to read-only for the following reasons: The project file has not been checked out of vault and I have open files in Inventor. Editing of a project file can only exist if no files are open in Inventor (and if you are using Vault, the project file is checked out). Next right mouse click on Use Style Library and change it to Read-Write.

      Hope this helps.


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