Being Inventive

Migrating content center libraries with custom materials to 2013

2012-05-17T17:47:41-07:00

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

Controlling the zoom speed of the scroll wheel of your mouse

2012-05-10T12:11:06-07:00

I bet most of us use a scroll wheel mouse as these type of mice are ubiquitous these days. So I wanted to share a tip with you all.
Generally I am a bit reluctant to share registry hacks as it could get you into trouble if you are not very careful when editing the registry.
But this registry hack is very useful. So it is hard to pass on not communicating this to the world.

There are probably two things you might want to configure as far as the scroll wheel goes: zoom direction and zoom sensitivity.

For the zoom direction we offer a convenient Application option on the Display tab that allows you to reverse the zoom direction.

This is very useful for users that switch regularly between AutoCAD and Inventor.

Fig 1: Controlling zoom direction in Application Options

For the zoom sensitivity we don't offer such a thing as an Application option and you either live with the default that we offer or you can change the value in the registry.
Here is the way how to do it for an Inventor 2013 installation.

Exit Inventor
Run regedit from the cmd window on the Windows Start menu
Locate following registry key HKEY_CURRENT_USER\Software\Autodesk\Inventor\RegistryVersion17.0\System\Preferences\Display\Wheel Zoom Speed
Change the value (default is 1). Changing to 0.1 makes the zoom 10 times slower. Changing to 10 makes it 10 times faster.
Exit regedit
Restart Inventor.

For older versions of Inventor change the version number string that I marked in red in the registry key.
Example:

17.0 = Inventor 2013

16.0 = Inventor 2012

15.0 = Inventor 2011

Etc.

Note: users that use a 3DConnexion device don't have to worry about all this as they can set zoom settings in the Properties dialog that gets delivered with the device.

Cheers

Bob

Inventor 2013 hanging on startup, check your Microsoft downloads

2012-05-10T11:34:05-07:00

Here is a tip from our Installation and Licensing team concerning Microsoft KB2633171.

Microsoft KB2633171 addresses some vulnerability issues in the Windows Kernel but adds the risk of more crashes on machines with ATI and Intel graphic cards.

And apparently also causes crashes of Inventor 2013…

So probably you will not be too sorry to see this KB go if it gives you back the chance to run Inventor 2013 J

For the full details, read the article on our UpandReady blog

http://upandready.typepad.com/up_and_ready/2012/05/inventor-family-hanging-on-the-splash-screen.html

Cheers

Bob

Controlling include/exclude state of components in Derived Assembly dialog box

2012-05-07T03:06:30-07:00

When you try to modify the state of Inventor assembly components in the Derived Assembly dialog box, you notice that some components cannot be included or excluded.

The Exclude button (second icon from the left) is grayed out.

This behavior is as designed.

The state (include / exclude) of components in the Bodies tab, depends from the visibility state in the Current Design View Representation if in the Representation tab the “Associative” checkmark is selected.

For example, an occurrence that is invisible is automatically set to the Exclude state and you are no longer able to include it in the derive operation.

To override the default settings and allow inclusion/exclusion of components without any interference of the Design View Representation, clear the “Associative" checkmark on the Representation tab.

This concept is similar to the one explained in this post, when the Visibility context command is disabled in a drawing.

In addition to this, in case you want to change the include/exclude state for some components that don’t show at all in the list, check the setting for the Level of Detail in the Representation tab.

In order to show these components in the list and change the include / exclude state, besides clearing the “Associative" checkmark, you need to set the LOD to Master or to another LOD where the components are not suppressed.

Ale

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

2012-04-30T03:00:00-07:00

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

Create your own Inventor tutorial

2012-04-26T13:42:36-07:00

I am excited to announce that the Learning Experience (LX) team at Autodesk has published a quick start guide on Autodesk Exchange that explains how to create your own Interactive Tutorial for use in Inventor 2013 and customize the Welcome Screen!!!

What this really means is that ***we just empowered our users to create new content****

When you search for "Inventor tutorial" on Autodesk Exchange, you will see this:

You can also browse directly to the download locations of the Inventor 2013 Interactive Tutorial Guide App on Autodesk Exchange

Click the Free button to download.

The App installs a Quick Start guide, an MP4 video, and two starter templates.

You can provide direct feedback on the App to: learning_app@autodesk.com

Be sure to give the App a review!!!

Thanks

Bob

Inventor 2013 literature for commuters

2012-04-24T14:12:43-07:00

Our learning experience team has released some interesting new PDF files, posted on the Help wiki.

This is information that was previously available in wiki and chm format but that now can be read at a more leisurely pace as a book on your laptop, PC or tablet.

It might be a good way of spending your time while you are on the go or while you are waiting for the plane, train, bus, taxi or rickshaw.

Here is a summary list of the new PDF.

What's New	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0000-What_s_N0#pageFiles
Inventor tutorials	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0127-Inventor127
Tooling	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0807-Tooling_807#pageFiles
Cable and Harness	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0904-Cable_an904#pageFiles
Tube and Pipe	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1042-Tube_and1042#pageFiles
Dynamic Simulation	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1111-Dynamic_1111
Stress Analysis	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1163-Stress_A1163
Frame Analysis	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1257-Frame_An1257

These files are bit awkward to find when browsing the wiki. You will have to scroll all the way down on their respective pages.

Here is an example of the location of the "Inventor Tutorials" PDF in the Files section at the bottom of the page.

Putting user parameters to work in part sketches in 2013

2012-04-24T14:02:33-07:00

When I heard about Inventor 2013’s ability to add custom parameters of both text and Boolean types I immediately thought it was a nice enhancement though I couldn’t really see a need to have something like an emboss show “True” or “False” in a part, but there may be a use for Boolean parameters in text that you’ll find and I’m overlooking. The next thought was there had to be a use for a Boolean with the text mixed with a little iLogic.

Here’s a very simple example of using a user text parameter and a Boolean parameter and put them to good use (and add the parameters to a part sketch without getting the “There is no parameter under this source” warning from previous versions)...

The first part is nothing new, just a matter of adding the parameters:

Sadly, you can’t send these parameters to a custom iProperty at this point as you can with a numeric parameter by checking on the export parameter box, right clicking and using the custom property format (as in d4 pictured below):

But what a delight to not see the warning when inserting the parameter by selecting the source as user parameters:

Now I can emboss and, voila, it’ll change when I change the parameter - immediately. The possibilities are starting to increase.

Now the only things left to do are 1) use iLogic to automatically control its visibility (incorporate the Boolean created) and; 2) since I’m already in VB, send the custom parameter to a custom iProperty – after first setting it to a null value so no warnings pop up the first time you run the rule. Why not as long as I’m already there, right? Now the catch here is I can set a string (text) value to null in VB or iLogic, but I don’t know how or if it’s even possible to set a Boolean value to null – just True or False to the best of my knowledge. But we can still use the Boolean to control whether or not the text value is visible with just a few simple lines:

And, now control the visibility of the emboss with that rule and the Boolean parameter:

I hope this helps you find more creative and complex ways to use this new functionality!

-Daren

Refresh material appearance in assembly parts in Inventor 2013

2012-04-24T03:00:00-07:00

You have changed the appearance of one material and saved the changes to the current active Material Library.

For doing that, you have set, in the active project, the option Use Style Library = Read – Write.

You have opened the Material Browser, for instance, in a part file.

Added the material to the document and displayed it in the editor.

You have applied your modification to the material appearance in the editor.

You have saved the changes in the current active Material Library from menu Manage > Styles and Standards > Save.

After doing that, you open an assembly that contains some components where you had applied the material you have edited afterwards, as explained above, and you want to update the appearance for these components.

In order to do that, in the assembly file, from the menu Manage > Styles and Standards, click on Update.

In the Update Styles dialog, select the active Material Library where you have saved your changes, from the drop-down menu and select the box Update Styles in all Child Documents.

Then, in the menu Manage > Update, click on Update Mass or Rebuild all, for getting the appearance update in the graphic window.

Ale

How to add a spot face symbol to your drawings

2012-04-20T10:37:53-07:00

We recently issued a hotfix to allow the use of custom fonts in hole notes. Right now the hotfix has been released for the Inventor 2010 Sp4 release only.

Note that thanks to this hotfix, 2010 users now have more powerful hole notes compared to 211, 2012 and 2013 users J.

But they will enjoy this exclusivity not for long. We plan to include the fix in the coming months in the service packs that we will publish for more recent releases.

Let me explain what this hotfix is all about so you understand the extent of its impact.

Without hotfix you are unable to add special symbols or character to a hole note unless you use the AIGDT font via the Character Map icon (see Fig 1).

Fig 1: Adding symbol from the AIGDT font via the Character Map

The AIGDT font suits most special symbol needs in the mechanical drafting arena, except for one particular situation.

It does not include a spot face symbol | SF | according to the ASME-Y14.5M-2009 drafting standard.

The spot face symbol is essential to distinguish a spot face hole from a counter bore hole.

Fig 2: Counter bore and spot face choices

Here is an example of a top view with seemingly two identical holes (if you just look at the hole notes)

Fig 3: Top view of two identical (?) holes

However when creating a section view, the holes look quite different.

Fig 4: Section view of the same holes

The hole on the left is a spot face hole and the hole on the right is a counter bore hole.

I admit that I artificially inflated the spot face depth to make it look more dramatic. But you will understand that there is a risk of misinterpreting the drawing by just looking at the top view and when no appropriate symbols are added to the hole notes. Here is where the above mentioned hotfix comes to the rescue. After applying the hotfix you can now select symbols from fonts other than AIGDT. You could even supply your own custom fonts.

If you include the spot face symbol as it can be found in fonts that are freely available on the internet (here is one example ASME-Y14.5M-2009 font), you get this result:

Fig 5: Addition of spot face symbol makes top view unambiguous

The only regret I have in all this is that we were not able to incorporate the same functionality in the style editor. This means that you won't be able to include the spot face symbol in a drawing template and that you will have to add the symbol on an individual note by note basis.

The other element to reckon with is that when you pack and go such a drawing to make sure that you also supply the special font to the party that receives your drawing. Otherwise they would not see the | SF | symbol.

But at least you have the power to create a hole note according to ASME-Y14.5M-2009 without waiting for Inventor to catch up with that standard.

Cheers
Bob