Being Inventive

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

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

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

Opening Inventor file opens new instance of Inventor

When you double-click an Inventor part file in Windows Explorer or in Vault Explorer, a new instance of Inventor opens even though the program was already up and running.

This is caused to an improper setting of the following Registry Keys :

HKEY_CLASSES_ROOT\Inventor.PartDocument/SHELL/open/command

Under this key the (Default) value should be showing the path to Inventor.exe with /dde at the end.

The value should be similar to this : C:\program files\Autodesk\InventorVersion\bin\inventor.exe /dde

HKEY_CLASSES_ROOT\Inventor.PartDocument/SHELL/open/ddexec

Under ddeexec, the (Default) string key should be set to: [open("%1")]

This is also valid for the other files types like Assembly which you will find under HKEY_CLASSES_ROOT\Inventor.AssemblyDocument\SHELL\open.

 

Inventor sets automatically these values on Start-up.

So, in order to solve the problem you simply need to log-in as Local Administrator of the machine and start Inventor.

Otherwise, with a Local Administrator user, modify these Registry Keys as explained above.

 

In case, after having applied the steps above, the problem still persists, in the registries, browse to

HKEY_CURRENT_USER\Software\Microsoft\Windows\CurrentVersion\Explorer\FileExts\.ipt

Delete the subfolder “UserChoice” from the above registry branch.

Repeat the procedure for any file type. Change extension as appropriate.

 

Thanks to Pierre Masson for the extensive testing he has done for this solution.

Ale

A new twist to shrinkwrap

On Autodesk Labs, we just launched a new app called Inventor Simplification with an improved and slightly different approach to shrinkwrapping specifically aimed at BIM workflows.
Check it out at: http://labs.autodesk.com/utilities/inventor_simplification/

Bob

Export parameters to iProperties as Numeric instead of Text Type

You have exported some parameters of your model to the iProperties Custom tab, selecting the Export Parameter check box.

The Type of the exported parameters in the iProperties is Text by default.

You want to know if there is a way to export them as Numeric Type instead.

In order to do this, in the Parameter list, right-click one of the exported parameters, edit the Custom Property Format and change the Property Type from Text to Number.

Besides, checking the option “Apply to existing comparable parameters” the change will be applied as well to the other parameters of the same type (Length, Volume, and so on), so you don’t need to change the Property Format for each parameter one by one.

Ale

Assembly document differences between FDS and PrDS

Note1: for a good understanding of this article, FDS stands for Factory Design Suite and PrDS stands for Product Design Suite.

Note2: to reproduce what is said in the article you will have to set your default File Open option for viewreps in the Application Options as follows:

The behavior that I will describe here has been bothering me for a couple of days before realizing what was going on.

So I wanted to highlight this to everyone to avoid unnecessary blank stares at the Inventor product J

Recently, while working in Inventor 2012 and also with the Inventor 2013 beta, I was confronted by surprise by the following dialog upon save of an assembly:

I had not seen this dialog before during save in a fresh new assembly after changing the color of one of the components.

The reason of course is that the Master viewrep is active and this viewrep is read-only (as is indicated by the lock symbol in the browser).

The cure is simple enough, like the dialog explains, to create a new view presentation to preserve the color changes before saving the assembly.

But I did not recall having seen the dialog in such a straightforward workflow. Here is what is going on:

There is a difference between the way FDS and PrDS create a new assembly document.

New assembly in FDS	New assembly in PrDS

 

In FDS 2012, the default viewrep is set to "Default" and thus is writeable. This behavior is independent from the viewrep option as set in the File Open options.

In PrDS 2012, the default viewrep in a new assembly is set to "Master" (and thus is locked) if "Master" is set in the FIle open options. This means that the PrDS File New behavior does depend on the File Open options which is unexpected and probably unwanted.

If you switch regularly between the two products, the difference in behavior between FDS and PrDS might confuse you.

But even for FDS users that stick to a single product but who temporarily want to simplify the ribbons by disabling the Factory add-ins, will at that point fall back to the PrDS behavior with the annoying dialog at save.

So don't tell me that I did not warn you J

Bob

Cannot select target assembly template in Make Components: Selection dialog

You have created a multi-body part.

Then, you go in the Manage tab, Layout and click on Make Components for creating an assembly with components from the solid bodies, but in the following Make Components: Selection dialog, the option for selecting the target assembly template is grayed out.

If you cannot select the Template for the Target assembly, it is because an assembly with the same name exists already in the location where you are saving it.

The behavior is as designed.

For instance, you want to add the components to an existing assembly, as explained in this post.

In this case, you don’t need to select a different template or BOM Structure for the Target assembly.

Instead, in case you want to replace the existing assembly, you have to click the icon for opening the Target assembly folder.

In the following Create dialog, click Yes for creating a new target assembly.

Select the assembly you want to replace.

And accept to replace it.

After that, the option for selecting the Target assembly template will be active.

Otherwise, if you just need to reactivate the option without replacing the existing assembly, you can simply change the Target assembly name in the dialog and the Template selection option will be available again.

Alternatively, you can click the icon for opening the Target assembly folder, in the following Create dialog, click Yes for creating a new target assembly and apply a new name for the Target assembly and / or select a different Target assembly location.

Ale

Part Number and Description always in synch for Frames

You want to insert the Structural Shape components in your assemblies in the way that in the iProperties, the Description Field value is equal to the Part Number one.

So, you have copied the Structural Shape Families you want to use in a custom library.

For each of them you have edited the Family Table adding a column with the properties as in the image below.

By the way, doing this you get the result you want inserting the Structural Shape components in your assembly with the command Place from Content Center

But not inserting them with Frame Generator.

In order to get the desired result inserting the components either way, you need to replace in the column property Expression “{PARTNUMBER}” with “=<Part Number>” as in the image below.

Ale

Change the default templates for the assemblies and parts created with Make Components

You have created some sketch blocks or solid bodies in your part file.

You want to create assemblies and parts out of them with the command Make Components, but you want to set some different from the Standard ones default templates for them.

You can change these settings in the Make Components Options dialog accessible from the Part Document Settings, Modeling tab.

From this dialog you can change also other default settings as you can see from the image above and read in more details in the WikiHelp under “Make components options”.

Of course, if you want, you can save these settings in your part template.

Ale

Inserting components using Composite iMates names

You have defined three Composite iMates in your component naming them A, B and C.

You have inserted this component in an assembly.

Now you want insert another component in the assembly and automatically position and constrain it to the first component using one specific Composite iMate.

For instance, you want to use for this purpose the Composite iMate A.

In order to do this, in the second component, you need to define the same Composite iMate, as the Composite iMate A of the first component.

The name of this Composite iMate is not important.

What is important is that the name of the Composite iMate A of the first component is in the top of the Match List of the second component Composite iMate Properties.

Once you have done this, you can insert the second component in the assembly where you have already inserted the first component selecting the option “Automatically generate iMates on place”.

You have to repeat the procedure for other components you want to insert using the Composite iMates B and C of the first component.

You can find more details in the video below.

Ale