Being Inventive

Associate by default materials to solid hatch in section views

You have an assembly view in your drawing.

You want to create the section view of it and apply automatically a solid hatch to the components with specific materials.

In order to do that, please follow the steps below.

• Download SOLID.zip and extract the PAT file in a location on your machine

• In the drawing file, open the Style Editor

• Select the Hatch style for the active standard

• In the right side of the dialog, open the drop-down menu for the Pattern and click on Other…

• In the following Select Hatch Pattern dialog click on Load

• In the following Load Hatch Patterns dialog, browse to the PAT file you have downloaded and load it

• After that, the solid hatch should be in the list of the loaded pattern and selected

• Click OK for closing the dialog

• Now the Solid hatch should be the default Pattern for the active hatch style

• Set the default Pattern back to the usual one (i.e.: ANSI 31) and save the Style edits

• In the Style Editor, select the active standard and in the right side of the dialog, select the Material Hatch Pattern Defaults tab

• Add the name of the materials you want to associate to the solid hatch
  • Alternatively, in the Import Materials section, you can import the materials from a part file, clicking on From Files… and selecting the part that contains the materials in the part document or from the active Material Style Library, clicking on From Style Library  

• Change their hatch Pattern from the drop-down menu and set them to Solid

• Save the edits in the Style Editor

• Then, create the section view of the assembly and get the solid hatch for the components with the specified materials

 

Final notes.

You can save these settings in the Style Library if you want to get the solid hatch associated to the specific materials by default in all the new drawings you create.

In case, after doing that you get the Style Conflict message opening a drawing template, read this post for solving the problem.

Of course, these settings apply also if you create the section view of a part with one of the materials specified.

 Ale

Environment variable "InvCM_ForceConvertToGeneric" to convert legacy colors to generic type in Inventor 2013

Inventor 2013 is using the Autodesk Material Library to provide a smooth appearance experience across the Autodesk Products.

However, you may see differences when migrating your files from older Inventor Release to the latest one. Bob wrote this Blog article  about the color topic in Inventor 2013.

In fact, the Autodesk Material Library was already available in Inventor 2012. You could access it in the Styles and Standard Editor, Field Realistic Appearance.
In most of the standard colors, the Realistic Appearance option was checked, but you had to enable the Realistic Appearance Mode to see it in the Graphic window.

 

Realistic apperance option and realistic visual style in Inventor 2012 

 

When migrating to Inventor 2013, you will see the realistic appearance. It might be looking differently than what you were seeing in 2012 classic shaded mode.
If you have standard colors in your 2012 document, they will get converted to our new 2013 standard colors (find the conversion table in Bob’s Article). So it will get another name and might look differently.

For example standard “Glass (Limo Tint)” becomes “Light Gray Reflective” in 2013.

The 2012 Colors style settings are no longer valid and we will use the realistic settings. You will see a much darker color shade, which matches what you would have seen in realistic mode in 2012.

Plus “Light Gray Reflective” will belong to the appearance category Glass/Glazing which has specific controls as you can see in the screenshot. Other categories will have other type of controls.

Glass Limo Tint in 2012 becoming Light Gray reflective in 2013

 

A new environment variable was provided in 2013 SP1.1 "InvCM_ForceConvertToGeneric" (value set to 1) that will maintain appearance names, ignore any realistic settings and convert all appearances to a generic type.

So if you migrate “Glass (Limo Tint)” with the variable in 2013, you will get a new appearance called “Glass (Limo Tint)” in the generic category and using the 2012 Color style settings.

 

 Environment Variable and Migration result of Glass Limo Tint with the variable

 

Usually the appearances in 2013 are darker, transparency can be different with the Glazing settings.
Use this variable if you want to minimize the difference between Shaded View in 2012 and Realistic Appearance in 2013. The appearances will be converted to generic type, which exposes all controls, and gives you more possibility to fine tune your visual results.

You will have to implement this variable on all your computers. Migrate once your custom library with the variable, and let the variable in case you get documents with local styles.

This variable doesn’t affect the materials.

Pierre.

Material Asset Missing

**** Update ******

The Inventor 2013 SP1.1 is now available here



http://usa.autodesk.com/getdoc/id=DL20442029

The Updated Service Pack will install on top of the previous Service Pack or the original release of Inventor 2013.

*********************

 

After installing the SP1 that has been temporarily retired as explained in this article, you can see this message popping up trying to add to the part document some materials from the Material Library.

If you are experiencing this problem, you need to uninstall the SP1, revert to Update2 and restore the backup copy of the Libraries (adsklib files).

If the corrupted library was migrated from a previous version and you don’t have a backup copy, you need to re-migrate the xml files.

By the way, even if you are not experiencing this problem, but, in your daily work you use to make operations like copy a modified material back to the library and use the replace option.

Or deleting Categories from the Asset Browser.

We recommend you to uninstall the SP1 and revert to Update2.

The updated SP1 will be available in the next days.

Migrating to 2013: materials and colors treated differently

I hope you have all seen this newsgroup post where we provide a PDF file explaining the mechanisms at play when migrating materials and colors to the 2013 release.

I have placed a copy of this PDF file here on our blog for your reference. The PDF file is a collection of Help wiki articles that are spread out throug the wiki.

Here is the list of wiki articles relevant to the style migration.

• FAQ Part 1
• FAQ Part II
• Data Migration > What's Changed in R2013
• Data Migration > Inventor 2013
• Data Migration > Migrate Color Styles to Appearances and Migrate Material Styles to Materials
• Data Migration > Migrating Content Center custom materials and appearances
• Manage Materials and Appearances
• 2013 Library Management Methods
• Migration Mapping – Materials
• Migration Mapping - Appearances

I wanted to make a couple of side-notes to all this.

First, before you start working with 2013, I would advise you to create a backup of the adsklib files and supporting files that came with the Inventor 2013 installation.

By default these files can be found in folder C:\Users\Public\Documents\Autodesk\Inventor 2013\Design Data\Materials

The reason the backup is not a luxury is because there is no easy way to restore a default material/appearance library in 2013, other than repairing your Inventor installation.

Your material library can also easily be altered by running an Update command on the library.
Coming to the main topic of this blog post, the other reason why you might end up with more materials in the material library than you expect is because materials are treated slightly differently than colors (appearances). Let me explain what I mean with that.

During migration, we change the color names and map the "old" colors to new appearance styles (here is a link to the appearance mapping table ).
For materials we don't change the material names during migration to 2013.
We decided to use a more conservative stance here because (contrary to colors) material names are exposed in BOM and parts lists and we did not want to change any existing parts lists during migration.

However when you create a new part from scratch in 2013, you will be using the new material names that differ quite a bit from the old names.
Here is a link to the new material names and how they relate to the old names.

Let me illustrate all this with an example. You can download the original 2012 data set here if you want to follow along.
Note that in this article I did not want to touch the subject of customizing materials. The sample file used for this article is using standard materials and standard colors as offered by Inventor 2012.

I created a part with

• Material = Galvanized Steel
• Color = Popcorn (the color is a rather outrageous color override for steel but it allows me to drive my point home later in the article)

Fig 1: Galvanized popcorn part in 2012

I create a drawing of this part and associate a special hatch style to the part material:

Fig 2: Custom hatch associated with Galvanized steel material

After migration to 2013 (simply reply Yes to any migration dialogs you might get), here is what you will see in the Quick Access Toolbar:

• Material= Galvanized Steel
• Appearance = *Nylon 6

Fig3: Same part migrated to 2013

This proves the point that the migration process changes the appearance name from popcorn to Nylon 6 but not the material name (although there is a suitable and similar material with name Steel, Galvanized available in the material library)

The * mark before the appearance indicates that Nylon 6 is not the default appearance that is normally associated with Galvanized steel.

What happens to our drawing after migration?

Here again the hatch style continues to be linked to the "old" Galvanized Steel material.

Fig 4: Galvanized steel material associated to ISO12W 100 hatch

There is no sign of the new Steel, Galvanized material until you hit the import material "From Style Library" button.

Only then are the "new" 2013 materials added at the bottom of the list (because of this the good news is that you can still distinguish between new and old :-) ).

Fig 5: Material list grows after pressing "From Style Library" button

Two things you can do at this point:

1. Do nothing and leave as is.
   This could create confusion between Galvanized steel and Steel, Galvanized both being present in the part and in the drawing.

   The other risk is that if you Update your cached styles to the library, you end up with both Galvanized steel and Steel, Galvanized in the library, hence my plea earlier to create a backup :-).

2. In the part, change the material to Steel, Galvanized and purge the Galvanized steel material from your document.

   
   

   Fig 6: Purging the "old" material.
   
   In the drawing, associate the custom hatch style to Steel, Galvanized.
   You can now get rid of the old Select Galvanized Steel material in the list and delete it with the Delete context menu.
   Repeat this for all old materials you no longer have a need for in the drawing. You can shift select to delete multiple materials in one operation.

   

   Fig 7: Associating the hatch with the proper new material

Method b) obviously results in a cleaner situation but it comes at the expense of more work, especially when dealing with many files.

Bob

Refresh material appearance in assembly parts in Inventor 2013

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

Style Conflict message

You start a new Inventor file (drawing, part, assembly, etc.), selecting one of your templates or the default one and get the Style Conflict message.

The error message is telling you that in the template file you have selected, the listed entities (i.e.: Layers: Center Mark (ISO), Standard: Default Standard (ISO) ) have different definitions compared to the same entities stored in the Style Library you are using in the active project.

As written in the message, the definitions from the Style Library will be used for these entities in the new file.

1. If you want to use the definitions from the Style Library when you use this template, but without getting the message every time you select it for creating a new Inventor file, do the following.

• Do not start a new file, but open the template browsing to its location (i.e.: C:\Users\Public\Documents\Autodesk\Inventor 2012\Templates).

• Menu Manage, Styles and Standards, Update.

• In the following Update Styles dialog, click on Yes to All and then OK.

• Click Yes in the following message and save the file.

 

2. Instead, if you want to overwrite the style definitions from your template file into your style library, do the following.

• In the active project set the option Use Style Library = Read-Write.

• Do not start a new file, but open the template browsing to its location (i.e.: C:\Users\Public\Documents\Autodesk\Inventor 2012\Templates).
• Menu Manage, Styles and Standards, Save.

• In the following Save Style to Style Library dialog, click on Yes to All and then OK.

• Click Yes in the following message and save the file.

By the way, if you decide to overwrite the style definitions from your template file (i.e.: Standard.idw) into your style library (Point 2), the next time you select this template for creating a new file, of course, you will not get style conflict message.

But, if you select a different template for the same file extension (i.e.: Standard_2.idw) for creating the file, you should get the style conflict message, because the second template should have the definitions from the Style Library before the overriding.

So, if you want to use the new definitions from the Style Library when you use this second template, for instance, if you want to use the style definitions you have saved from Standard.idw into the Style Library in Standard_2.idw as well, but without getting the message every time you select it for creating a new drawing, you have to apply the procedure of Point 1 above for the second template.

 

3. If you want to use a different style definitions than the ones from the Style Library but just with a specific template, in previous versions you could set the option Use Style Library = No in the active project.

This option is not available in R2012.

You can find more details here about why this option has been removed and a procedure if you want to use the cached style definitions of your template anyway.

Ale

Interference Edges and Hidden Lines

You have created the view of your assembly.

Then you show the hidden lines for all or some components and select to display the Interference Edges as well.

 

After that, you notice that unexpected lines occurred in the view.

 

The lines that show up are Hidden Interference Edges.

If you don’t want to see those lines, in the Style Editor, create a new layer and turn it off.

 

Then, in the Object Defaults, map the Hidden interference to that layer.

 

Ale

Default setting for the option “Use color override from source component” in the Derive Part dialog

When you derive a part in Inventor 2012, in the Derive Part dialog, the option “Use color override from source component” is grayed out and selected by default.

So, if you want to apply a different color style to the derived part, you need to select the derived node in the derived part browser and uncheck the option.

 

 

The same applies when you mirror the components in an assembly or when you create them using the Make Components functionality in a multibody part.

In these cases, the option is not available in the Mirror Components or Make Components user interface.

So you need to edit the derived node of each individual derived part where you want to apply a color style different from the source part.

 

If this is a common daily workflow process, you can disable the option “Use color override from source component”, by default, following the steps below.

Before following the procedure, you need to install the SP1 for Inventor 2012, if you have not done it yet.

 

 

• Close Inventor.
• On the Start menu (Windows), click Run.
• In the Run dialog box, enter REGEDIT.
• In the Registry Editor, locate the following key and export it:

HKEY_CURRENT_USER\Software\Autodesk\Inventor\Regis​tryVersion16.0\System\Preferences\PartDerivedPartD​lg

 

• Save the reg file on your machine and name it, for instance, “color_override_on.reg”.
• Extract the reg file from the Color_override_off.zip file on your machine, double-click on it and accept to change the registry settings.
• Restart Inventor.

Notes.

The new setting applies just to the new derived parts you create after applying it.

If you want to go back to the previous default setting, you need to close Inventor, double-click on the file “color_override_on.reg” you have created in the step above and restart Inventor.

 Ale

Fix hatch angle in section view

When you do cross section view on an assembly in drawing mode, the hatch angle is assigned automatically.

 

If you want to fix it either for 45 or 135 degree,

• Edit the Standard in the Style and Standard Editor.
• Select "Section Hatch Angle" in the dropdown.
• Remove all values, but 0 and 90.

 

 

Ale

Inventor Colors and Priority Order

In Inventor, we have several types of colors

Instance color—assigned on the components in assembly environment.

 

Face Color—assigned on Face directly: right click on one face, choose Properties and then you can change it.

 
 

Feature Color—assigned on Inventor feature directly: right click on one feature, choose Properties and then you can change it.

Note: one feature contains several faces.

 

Body Color—assigned on body directly: right click on one body, choose Properties and then you can change it.

Note: one body may contain several features.

 

Part Color—assigned on the whole part directly: choose the color settings directly.

Note: one part may contain several bodies.

 

The priority order is the following:

1. Instance color
2. Face color
3. Feature color
4. Body color
5. Part color

That is, if you have face color and body color assigned on one body, the body will present the face color for the specific faces, while others unassigned will present the body color.

In the image below, Red is face color, Blue is feature color and Brown is body color.

 

Ale