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.

 



Dragging in Inventor is Everywhere

In many Inventor command functions you have the opportunity to enter a function value or you can show Inventor the value by left clicking and "dragging" the displayed arrow.  In this article I hope to show you how to make this function as productive as possible.  Below is the extrusion command function that presents a "dragging" value entry.  You would simply left click the arrow and drag to the desired value.

Most all command functions which ask for a value also offer the drag arrow.  The commands cross both modeling and editing functions but depending on your configuration settings, you may not be getting the most from their use.  So I would like to talk about that first.  When I was a machine designer, my CAD manager told me to always design one, to use stock size materials when possible and two, when I had to machine cut material shoot for full inch dimensions, then halves and quarters of an inch.  He made it clear he did not want to see any eights or smaller of an inch unless it was necessary.  Of course we were a high tolerance machine builder and some dimensions had to be in the thousands of an inch and even ten thousands for special fits.  He believed using the largest inch division possible would speed shop production and I must say he was correct.  Just think how sending a piece of structural steel to the saw operator with a non-critical length as 36 47/64 inches instead of 36 3/4 inches would slow him down.  Sure he would probably cheat and round it but you never know.  

The configuration should be done in your companies part and assembly template files so it is available for all designs.  I will be using an inch part template but the same ideas applies to metric templates.  Open up the part template and on the Options panel under the Tools tab select Document Settings.

Select the Modeling tab in the Document Settings dialog box and enter your 3D Snap Spacing for both distance and angle dragging.  This will automatically keep the entry value to increments of the value you enter when you drag a function arrow.  In my case I have set 1/8 inch distance which will quickly give me enough accuracy for non-critical modeling but will also allow me to easily conform to my CAD manager rules just using the drag function, without keyboard entry.

I did not mention it but if you left click and drag on the ball at the base of the arrow, you can "drag" enter angle values in increments of the above setting, in my case 5 degrees.  This is not available in all functions.

Once you have saved your template, your next part or assembly model it will be easy to "drag" the value of your next extrusion, revolution or fillet radius just to mention a few functions.  Of course you can always over-ride the drag value by typing in an value you desire.

So that covers modeling functions but how about sketches.  You can accomplish the same thing in your Inventor sketches by configuring the Snap Spacing under the 2D Sketch section under the Sketch tab in the Document Settings dialog box.  Of course this should also be done in the part and assembly templates.  There is no setting for an increment angle.

There is one more configuration that needs to be set to allow 2D sketch snap spacing to work.  This is done in the Application Options dialog box located on the Options panel under the Tools tab.  On the Sketch tab, place a check mark beside the "Snap to grid" option.  You do not have to turn on the grid display, located in the same dialog box, unless you desire to have a visual grid during sketching.

You will get an odd readout when you are sketching lines at an angle if your Heads-Up-Display Dimension Input is set to "Polar Coordinates".  It is actually snapping to your snap settings but since it is on an angle, the values displayed are not intelligent.  If you change your Dimension Input to "Cartesian Coordinates", the values will display increments of your settings.  I do not believe this is an efficient setting but that is a personal opinion.

So give the Inventor dragging options a try.  If you would like to test before changing your default templates, make the configuration changes in one of your parts using your current template.  If you like them, transfer the settings to your default templates.

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!