Being Inventive

Error 1328. When Applying Vault 2012 Update 1

During the installation of Vault 2012 Update 1 (Autodesk Vault 2012 Update 1 (Client).msp) you see this error.

Error 1328. Error applying patch to file C:\Config.msi\XXXXXX.tmp. It has probably been updated by other means, and can no longer be modified by this patch. For more information contact your patch vendor.

This is caused by a problem with the "Connectivity.Branding.Vault.dll" file and reports indicate that this particular message is only occurring with plain Vault installed from one of the new suites. The dll is not present with the licenced versions of Vault and so we have no reports of this happening with Vault Workgroup, Collaboration or Professional clients.

UPDATE 02/11/2011

We have reproduced this internally and Autodesk is working on a solution that avoids the problem. Initially a solution was identified to replace the above mentioned dll with another version, However this could have unforeseen side effects and we would suggest that you wait until a formal solution is in place. We appreciate your patience.

We also are seeing reports of a different install error occurring with the licenced versions of Vault, but with different dll files. So far have not reproduced this internally. If you are experiencing the issue with a different dll, please log a support case with Autodesk.

Update 30/11/2011

This issue should be addressed by ts18131263

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Licensing: Autodesk Product Design suite Premium 2012 Package License, AutoCAD Mechanical 2011 and Inventor 2011 takes 2 licenses

If you have Autodesk Product Design suite Premium 2012 Package license and if you still use 2011 version of AutoCAD Mechanical and Inventor, you might find that it is using 2 seats (if you have more than 1 license) or for you get license error for the second product.

One work around to the issue is to make sure the Inventor 2011 is started prior to starting AutoCAD Mechanical 2011.

If you don't want to pass on the responsibility to the user then you can create an option file with the following line to exclude AutoCAD Mechanical 2011 to all the users, forcing the users to checkout Inventor 2011 feature code.

INCLUDE 85545AMECH_PP_2011_0F USER DUMMYUSER

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Creating iLogic rules automatically

After days of laborious work to create yourself the golden iLogic rule that your company cannot live without, the realization suddenly strikes that your golden rule will only work on newly created files.
How can you retrofit an iLogic rule to already existing files?
In iLogic, there is not such a thing like "automacros" such as in VBA macros.
How do you avoid having to paste your iLogic code manually in each and every file?

External rule anyone?

A piece to the solution of this puzzle is to use an external rule.
An external rule has one big advantage over a local rule.
It can be modified in a single central location while still affecting all files that call that external rule.

Calling an external rule in iLogic is very simple:

    iLogicVb.RunExternalRule("externalrule.txt")

To focus attention, let's do something very basic in the external rule like bringing up a message box that displays the filename.

The rule in externalrule.txt to accomplish this, would be

    MessageBox.Show( "File name of active document is " + Chr(13) + ThisDoc.PathAndFileName(True), "File name" )

But how can you get this one-liner systematically included in existing files?

API coming to the rescue

You can achieve this by using the AddRule command from the iLogic API as documented in the file called "Autodesk.iLogic.Interfaces.xml".

This file is located in the Inventor bin folder if you like to dive in for more details.

To put it all together, I created a VBA ivb project and an external rule. Both files are all you need to make it work and can be downloaded here.

Here is the procedure to use the files. It is important that you follow all these steps without skipping any.

1) First unzip the ivb and txt files to any folder. Example: C:\Shared\myivbprojects

2) In Inventor Tools > Options > iLogic configuration and add the name of your folder to the external rule directory paths.
Note : this command sits in the expanded panel by default, so it is rather difficult to find.

 

Figure 1: Adding location of external rules

3) Load the ivb project in the VBA editor via File > Load project ...

4) Run the macro initialize_iLogic_rule() in module Start_stop

5) Create a new Inventor file or open an existing file (if you want to treat multiple files you can also drag and drop files from Windows Explorer to Inventor)

6) An iLogic rule called "Myrule1" will be automatically created (if you run the rule you will see that it will try to display the filename)

7) Do not forget to turn off the automatic rule creation process if you no longer need it. You can do so by running the macro called stop_initialize_iLogic_rule() in module Start_stop.
Step 7 is really important if you want to stop adding rules automatically.

Extrapolation to more rules

Above code is dealing with a single external rule. What if you want to add multiple rules in one operation?

For example if you want to add a second rule, you will have to change just a single line of code and make sure that the extra string you provide matches the external file name Myrule2.txt  etc:

   

To create two rules simultaneously, modify this line

listofrules = Array("Myrule1")    

By adding an extra string    

listofrules = Array("Myrule1", "Myrule2")

Make sure that the external rules with corresponding names exist:

Myrule1.txt , Myrule2.txt  , etc

Now if someone can find the trick to automatically set triggers to run rules then we would have a complete automated solution … Anyone out there?

Have fun

Bob

BOM Structure of Content Center parts

You have copied some standard part families of washers and bolts from the Content Center to a custom library.

Now, you want to change the BOM Structure of these standard part families, for instance, from Purchased to Phantom, because you don’t want these standard parts showing up in parts lists.

Of course, you can use the Parts List filters for this purpose.

But you prefer not to just shut off the visibility at that level. 

In this case, in order to change the BOM Structure for a Standard Part Family, you can do the following.

• Copy the Standard Part Family to a custom library, if you have not done it yet.

• Open from Content Center.

• Open any component from the family with the “As Custom” option.

• Save the file to your local computer.
• Click Tools menu > Document Settings.
• On the Bill of Materials tab, change the Default BOM Structure from Purchase to Phantom.

• Click Apply and then Close.
• Close and save the file.
• In the Content Center Editor, select the custom library in the Library View field.
• Right-click the family. Click Replace Family Template.

• Click Yes in the following dialog, select and open the file saved in the step above. 

• Click OK in the “Publish was Successful” dialog box.

You need to repeat the procedure for each Standard Parts Family of which you want to change the BOM Structure.

Ale

Parts Only and Structured Parts Lists in one drawing

You want to have a Parts Only Parts List and a Structured Parts List in one drawing.

For instance, you want to have the structured list to show the assemblies as well as a parts only list to show common parts between the assemblies.

You can get it following the steps below.

• Create the main drawing with a Structured Parts List or a Parts Only one in it.
  • The Parts List schema you use at this point is the one represented by the balloons if you insert them later on, having the other Parts List schema as well in the drawing.

• Create a new drawing.
• Insert the other Parts List schema in this second drawing.
  • That is, if you have inserted the Structured Parts List in the main drawing, you have to insert the Parts Only Parts List in the second one, and vice versa.
  • You don’t need to create an assembly view in the second drawing; just select the assembly and the desired schema in the dialog.

• Copy the Parts List in the second drawing and paste it in the main one. 

Ale

Detect mass overrides in large assembly

You want to detect in a large assembly which of the components have mass properties overrides without opening each and every component.

In order to do this,

• Download and unzip this VB File to your local drive.
• In Inventor, menu Tools > VBA Editor > menu File > Import File and select the file BomOverrideQuery.bas.
• Open the main assembly.
• Run the macro called BomOverrideQuery.

• A txt file is created and you get a message with the path where the file is saved.

• If a mass override has occurred for some component, you will see the word "Yes" in the last column of the txt file created.

Working with Large Assemblies WikiHelp page

We have created a WikiHelp page related to working with large assemblies in Inventor.

We’ve combined several white papers, training documents, and other documents to create this resource.

We encourage you to not only reference this page to help with your Inventor designs, but also contribute to it with your experiences and workflows.

We hope you find it useful.

Grips not available for some entities in AutoCAD Mechanical 2012

You have installed AutoCAD Mechanical 2012 and SketchBook Designer 2012 on your machine, for instance, from the Product Design Suite media.

In AutoCAD Mechanical you notice that, selecting some entities, the grips don’t display

Even if the option for display them is selected.

The problem is due to SketchBook Designer for AutoCAD 2012 AddOn.

Our development is working for fixing the problem.

In the meantime, in order to display correctly the grips, you need to start Mechanical without loading the SketchBook Designer AddOn.

For doing this, follow the procedure below.

• Close AutoCAD Mechanical 2012
• Browse under the folder C:\Program Files\Autodesk\ApplicationPlugins and locate the folder named SketchBook Designer.bundle.

• Rename the folder, for instance, as SketchBook Designer.bundle_unload

• Restart AutoCAD Mechanical 2012.

After that, the grips display correctly and the SketchBook Designer AddOn is unloaded.

If you want to load the AddOn again, restore the original folder name SketchBook Designer.bundle and restart Mechanical 2012.

Of course, the grips display problem will be back as well.

Ale

Center of Gravity and Level of Details

You have created an assembly view using one specific Level of Detail created in the assembly model.

Then, selecting the assembly under the view in the browser, you select to display the Center of Gravity from the contextual menu.

 

The position of the Center of Gravity, by the way, is the one of the Master LOD and not of the one you have used for creating the view.

 

This behavior is “as design”. The Center of Gravity only refers to the Master level of detail representation of the assembly.

LOD is a memory management tool. Although you don't see certain components in a LOD, they still contribute to the mass properties and the CoG.

If you want configurable assemblies with configurable CoG, use iAssemblies instead of LOD.

 

Alternatively, you can use the following iLogic solution.

• Download and unzip this ILogic Rule to your local drive.
• Create an iLogic rule in your assembly, using the script you have downloaded.
• Trigger it on "Save" and for "Component Suppression changes".

 

• The rule creates/updates a workpoint called "Center of Mass" at the CoG of the active assembly LOD.

 

• In the drawing view, uncheck the "Center of Gravity" option.

 

• Recover the workpoint in the drawing view by using "Include work features...".

 

• And get the desired result.

 

Adding Parts to Top Down Assembly

You have created an assembly selecting some bodies from a multi-body part.

 

 

 

Afterwards, you want to add more parts to that same assembly from other solid bodies of the original part you have not selected when you have created the assembly, or that you have created in the original part after creating the assembly.

For doing this,

In the Make Component dialog, select the other solid bodies.

 

In the Target assembly name field write the name of the assembly created previously.

 

Ale