Being Inventive

Empty Part Number for Content Center Library components

When you insert a component from a Content Center Library family either with the command Place from Content Center or with Frame Generator you want that the Part Number field is empty.

In order to do that,

• Copy the family in a Read/Write library

• Select the family you have copied, right-click, Family Table.

• In the Family Table, select the Part Number column, right-click, Column Properties.

• In the Column Property dialog set the Expression Column field to “=”

• Publish the changes.

After that, inserting a member of that family either with the command Place from Content Center or with Frame Generator you will get an empty Part Number field.  

Note. If you have modified a Structural Shape family as described above and you generate the members with Frame Generator, you need to select the box "Get Frame Member's Part Number from Content Center" in the Insert dialog for getting the empty Part Number for the frames.

By the way, the box is checked by default.

For more information about this option you can read this post.

Ale

Override the appearance for the members of a Content Center Library family

When you insert a standard part from the Content Center Library, the color of the part corresponds to the appearance associated to the material.

That is, if, for instance, the material set in the family table is “Still, Mild”, the color of the part will correspond to the appearance of this material in the active material library (i.e.: Steel).

If you want to override the appearances of the family members when you insert them in your assemblies, you can do the following.

• Copy the family in a in a Read/Write library.

• Add a new column in the Family table.

• Assign a name to the column and map it to the “Member.Color” Inventor property.
• If you want to override the default (material) appearance with a different one that is the same for all the members of the family, check the Expression box and write the name of the desired appearance in the Expression field.

• Otherwise, if you want to apply different appearance to each member or group of members, leave the Expression box unchecked and fill up the cells of the new column for each member with the appropriate appearance.

By the way, in both cases, the names of the appearances you write in the Expression field or in the new column cells must match the names of the appearances from the active Appearance Library.

Ale

 

Place a Tube & Pipe fitting in an assembly as a normal part

You have opened a Tube & Pipe fitting from the Content Center using the option “As Custom” and saved the file in a location of your machine.

Then, you have inserted the file you have saved in an assembly with the command Place Component, but the file is still behaving as a Tube & Pipe fitting.

For instance, if you right-click while inserting the component, you get the same context menu as if you were placing the fitting in a Tube & Pipe subassembly.

In the assembly browser the fitting icon is the same as if you have inserted the component directly from the Content Center.

The component cannot be demoted, etc.

This behavior is as designed, because the fitting still contains the authoring information that, for instance, would allow you to insert and connect it to a Tube & Pipe run.

So, if you want to insert the component as a normal part, after you open it from the Content Center using the option “As Custom”, you need to remove the authoring info stored in the part with the code you can find in the solution http://usa.autodesk.com/getdoc/id=TS13404549

After doing that, inserting the component in an assembly, you won’t get the Place Fitting context menu, the icon in the browser is the same as a normal part that, in case, can be also demoted, etc.

 

By the way, the fitting still has some Content Center properties as you can see from the context menu, right-clicking the component.

If you want to copy or mirror the fitting along with other assembly components and standard parts and the option “Reuse Standard Contents and Factory Parts”, this can be just reused or excluded.

So, if you want to remove any trace of the Content Center properties, you can use this Macro before inserting the fitting in your assemblies.

Of course, you can easily combine the two macros if you need to remove both authoring information and Content Center properties from the fitting before inserting it as normal part in your assemblies.

Ale

Vault Check In Error and Content Center Language

You are working with a Vault project and while checking in an assembly with its components you get the Check In Error below related to some Content Center standard parts.

In general, this error that prevents you from checking in the assembly is due to two contributory causes

The first one is the Vault setting “Enforce Unique File Names”.

This is a very common setting for most of the Companies using Vault.

 

The second cause is when the Inventor users, sharing the common Vault project, use Inventor in different languages.

In general, when this is the case, the users don't change the Content Center Language, that is the same of the product they are using by default.

By the way, when users that share the same project use Inventor in different languages, it is recommended they configure the Content Center to use the same language.

If they don’t do that, you can read below the details of a possible scenario that can lead to the Check In error.

 

A Content Center standard part resides in Vault because it has been inserted and checked in by an user, using the English language for the Content Center.

Another user inserts in another assembly the same standard part from the Content Center.

If this second user uses the same language for the Content Center, the standard part will be retrieved from Vault.

So, there is no problem checking in the assembly, because the standard part will not be listed in the files to be checked in.

Instead, if the second user is using a different language for the Content Center (i.e.: German), the standard part file will be created under the subfolder related to the Content Center Language (i.e.: C:\Users\<user name>\Documents\Inventor\Content Center Files\R2013\de-DE\DIN 404(1)) and it will not be retrieved from Vault, because the folder structure is different.

So, when you check in the assembly, Inventor will try to check in also this standard part and you will get the Check In Error because actually a file with the same name is already in the Vault.

 

By the way, if this is your case and you are stuck because you cannot check in your assembly you can follow the steps below for solving the problem.

• In Vault Explorer check the Content Center language the other users are using for inserting the standard parts in the assemblies (i.e.: en-US = English).

• In Inventor (without closing the assembly you cannot check in), menu Manage > Content Center > Editor.

• In the Content Center Editor, menu Tools > Language Setting and set the language as the other users > Done.

• Menu Manage > Content Center > Refresh Standard Components.

• All the standard parts inserted with a different Content Center Language will be listed and refreshed.

• After that, save and check in the assembly.

No error message will appear this time.

Ale

Content Center File Versions

By default Inventor creates sub-directories related to the version you are using (i.e.: %USERPROFILE%\Documents\Inventor\Content Center Files\R2013\) in order to store the generated Content Center instance files.

If you have never changed this behavior, one of the consequences you can see is that you can generate the same content center instance in multiple directories, inserting, for instance, the same component with Inventor 2012 and then with Inventor 2013 when you upgrade to this version.

Another issue you can experience using the same project after having upgraded your Inventor version, is getting the Resolve Link dialog related to some content center parts, when you open an assembly created in the previous releases.

So, you want to migrate all the content center files in those directories to your current release (i.e.: 2013) and place them in a common "generic" directory without separation into yearly subdirectories and using this location without problems when you upgrade to the next Inventor version.

After you have applied the procedure below, you will get that, having all the content center files you have inserted in the assemblies of your project updated to the latest version and without getting any Resolve Link dialog opening any assembly of the project

• In Inventor, menu Tools > Options > Application Options > File tab, set your generic path (i.e.: C:\Demo) in the Default Content Center files filed.

• Close Inventor.
• In Windows Explorer open the default Content Center file location corresponding to the oldest Inventor release you have used for inserting the Content Center parts (i.e.: C:\Users\<user name>\Documents\Inventor\Content Center Files\R2010).
• Copy the subfolder en-US with its content and paste it under the new Content Center File location (C:\Demo).

Note. If you are using Inventor and / or the Content Center in another language, the name of the subfolder to copy is different (i.e.: de-DE for German, fr-FR for French, it-IT for Italian, etc.)

• After that, in Windows Explorer, copy all the folders located under the en-US subfolder under the default Content Center file location of the next Inventor release (i.e.: C:\Users\<user name>\Documents\Inventor\Content Center Files\R2011\en-US) and paste them under C:\Demo\en-US.

• While doing that, in case, accept to merge the folders with the same name and to replace the files with the same names with the newer versions.

• Repeat the two steps above for the next Inventor versions (i.e.: 2012 and 2013).
• If you were using custom libraries in previous versions and you want to migrate and use them in the latest Inventor version as well, you can follow the procedure you can find here for migrating them.
• If you were using custom materials in your custom content library, you need to migrate your custom material style first as explained in this post.
• Otherwise, if you were just using the Standard CC Libraries without any customization, you can skip the previous two points.
• Once you have copied everything under “C:\Demo\ en-US”, in order to update all the standard contents to the latest Inventor versions, start Task Scheduler, menu Create Tasks > Refresh Standard Components.
• Select your project, select the “Immediately” checkbox and click OK for starting the process.

• When the process is complete, you can open the log file for checking if it succeeded

In the video below you can see some of the key points above in action.

For demo purpose the video has been created using a small data set, but I hope it could be useful for clarify the procedure even if you want to apply it to a large data set.

Ale

Migrating content center libraries with custom materials to 2013

I wanted to make everyone aware that due to the new way of working with materials and appearances/colors in 2013, extreme caution has to be observed when migrating custom Content libraries that contain custom materials.

The order in which you do things is of utmost importance. The proper migration order is:

1. Migrate your custom material style into a 2013 material library first

2. Make sure that the proper material library is active in your project file

3. Update the content center library

 

I'll give a more detailed example of each of these steps.

Assume that I have a Content Center family defined in a desktop content file Mylibrary.idcl that uses a material called "Glowing red uranium".

Why uranium? I like to live dangerously J

Fig 1: Custom Content family with Custom material

I'll describe two possible scenarios.

Scenario 1: the custom material is defined as part of your Materials.xml and Colors.xml file in 2012 and you want to migrate the custom material into the existing InventorMaterialLibrary.adsklib library.

Scenario 2: the custom material is exported in 2012 as an individual style file called glowingred uranium.styxml and you want to migrate this style to a brand new 2013 Material library.

Step 1. Migrate the custom material style to 2013

This can be done quite easily by using the Migrate Inventor Styles option at the bottom of the Material editor window.

The only downside is that you will need to start a new Inventor part or assembly file to gain access to the Material and Style editor.

Scenario 1:

Start a new part and start the Material editor

Start the Migrate Inventor Styles command

Fig 2: Location of the Migrate Inventor Styles command

Select as origin location the folder where your Materials.xml and Colors.xml file sit.

Select as destination location the folder of the InventorMaterialLibrary.adsklib , which is by default in C:\Users\Public\Documents\Autodesk\Inventor 2013\Design Data\Materials.

Fig 3: Migrating material style to existing 2013 material library

Close and reopen your Material editor and you should now see the custom material show up in the list

Fig 4: Custom material correctly migrated

Scenario 2: if you have an individual file glowingred uranium.styxml that you want to migrate to a new library.

First create a new material library and call it Mylibrary.

Go to the Style editor and Import the style

Fig 5: Import button allowing more granular style migration

If you open the Material editor, you will see that the imported material is showing up in the top portion of the dialog, indicating that the material is cached as a local style in the active document.

Fig 6: Locally cached material style

This means that our custom material is not in the library yet. To get it in the library, you would have to explicitly tell Inventor to add it to our library with the "Add to" context command.

Fig 7: Adding a custom material to a new library

This brings us to step two which involves some work in the active project file.

Step 2. Make sure that material library is active in your project file

Close all documents and open the project editor

For Scenario 1: make sure the Inventor Material Library is the active library

For Scenario 2: add the Mymaterials.adsklib file and make it the active material library (in bold)

Fig 8: Verifying in the project editor that the custom library is active

Step 3. Update the content center library

Keep your project file open and add the custom content center library (mylibrary.idcl) by clicking on the lower right icon in the editor.

The library will be flagged as being out-of-date by showing a yellow exclamation mark.

Fig 9: Warning sign that My Library is out of date

 

Hit the update button at the lower right of this dialog and you are set.

 

To fully test that your content center library works correctly, start a new assembly and place a part from the "My Library" library or you could also check the material in the content center editor of course.

 

Hopefully above procedure will spare you some headaches.

The bottom line is:

Please make sure that your custom materials are migrated correctly BEFORE hitting that update button in step 3.

Migrating the custom material to 2013 after the content center library has been updated to 2013, does not work unfortunately.

 

Thanks

Bob

 

 

Create linked copies of a Content Center family with different materials using the Material Guide

You want to create copies of a standard family in Content Center.

You want each copy to have a different material.
In addition you want that any change you make to the first copied family will apply to the other copies as well.

In order to achieve this, all copies need to be linked to the first copied family.

So, starting from one standard family and using the Material Guide, you need to create first an independent copy with a different material.

Then, from that family copy, with the Material Guide, create the other copies linked to parent family and assign to each copy a specific material.

You can see the procedure in the video below.

Ale

Edit Custom Property Format for a standard part parameter

You have copied one Standard Family in a Read\Write Library.

You have modified the Family Table to include a parameter in a custom property, as explained, for instance, in this post.

By the way, you don’t want to display, Trailing Zeros, Units String, etc., for this parameter in the custom property.

In order to avoid that, do the following.

• Open one component of the Family with the option “As Custom” and save the file on the disk.

• In the file parameter list, select the parameter, modify its Custom Property Format, removing, for instance, the Trailing Zeros, Units String and save the file.

•  In the Content Center Editor, Replace Family Template selecting the modified component.

After that, inserting one family component either with Frame Generator or from the Content Center, the parameter will display as expected in the custom property.

Ale

Include the length from the Steel Shape profile in a custom property

When you insert the Structural Shapes with Frame generator, for each frame you want to have a custom property displaying its length along with other properties (i.e.: Stock Number).

In order to do that, you need to do the following.

• Copy the Structural Shapes family in a Read/Write library.

• Add a new column in the Family table.

• In the Column Properties define the Expression as “={STOCKNUMBER}&-&<G_L>”.
• Map the Column to the Custom Property and assign a name to it.

After doing that, you will get the profile length in the custom property either when you insert it, with Frame Generator or from the Content Center, and the length value will update accordingly, if you edit the frame.

You can see all the details in the video below.

Ale

Supplier Content Center link is broken

On this and others Autodesk pages, we have a link to http://www.autodesk.com/suppliercontent

Since few days, all these links are being redirected to http://mosaic.autodesk.com/inventor (a labs site).

We are working for fixing the links and those should be restored soon.

In the meantime, you can use the link below to get the correct location of the supplier content.

http://autodesk.partcommunity.com/portal/portal/autodesk/PARTcommunity/Portal/autodesk