Being Inventive

You’d like to see the volumes for all of the members of an iPart at once

This came up recently with a customer where they’d like to see all of the different volumes at one time for an iPart’s members. This could be used for mass or other property. The only limitation is your creativity with it.

The scope is: we want to get the volumes for all the elaborated members of an iPart factory at one time and this rule does that when we add a custom “Volume” parameter to the iPart table, trigger the rule to fire on any parameter change and edit the table via a spreadsheet. Problem: Cubic inches (or any other distance type) doesn’t have a predefined enum.  So we need to use a workaround and build up a string that defines the desired units.  There is the issue of the unit type changing from document to document so we won’t want to hard-code the unit value but instead be able to set it dynamically. We also want to make sure that, if the parameter exists, we’re not duplicating it and it’s correct for the current member. Here’s how the code looks:

'Dimension a variable for user paramaters

oMyParameter= _

ThisApplication.ActiveDocument.ComponentDefinition.Parameters.UserParameters

'test to see if the parameter is already there and, if so, that it matches the correct

'volume of the member using the embedded if/then/end if block

Dim param As Parameter

   On Error Resume Next

   param = oMyParameter.Item("Volume")

   If Parameter("Volume") <> iProperties.Volume Then

   Parameter("Volume") = iProperties.Volume

   End If

   On Error Goto 0

'If it doesn't exist, create it so that we can add it to the table. We have to concatenate

'Units of measure as a string b/c there is no enum for ^3 inches but no problem, it still

'can be had and dynamic the way we'll set it up

If param Is Nothing Then

'Get the document's units of meausure, comcatenate that with a volumetric string of ^3

'in order to show the units as volume units

Dim uom As UnitsOfMeasure = ThisApplication.ActiveDocument.UnitsOfMeasure

Dim volUnits As String = uom.GetStringFromType(uom.LengthUnits) & "^3"

'Set a parameter equal to the current properties volume adding the units of

'measure in volume units from above

Dim Vol = iProperties.Volume

oParameter=oMyParameter.AddByExpression("Volume", Vol, volUnits)

End If

iLogicVb.UpdateWhenDone = True

‘Then, once this rule is run, it’s just a matter of adding the new “Volume” user

‘parameter column (from other) we’ve created to our iPart table – just once.

I’m sure there are probably other ways to do it but it really works out pretty well with very little actual code. As a note, when you change members, you’ll get a dialog that you should answer yes to, that states the values in the active row do not match. It is asking you if you'd like to update the table with the new value before continuing. Answering yes will reflect the volume for the new member's cell value in the table in both the iPart table in Inventor as well as in the Excel spreadsheet.

Once they've all been activated and the dialogs have been answered "Yes", your values will be reflected in the table/spreadsheet.

 

-Daren

 (1st line of code edited with underscore to fit in the provided space)

Copy Active Camera View to all Opened Documents

You might want to compare how different components look like from a specific point a view. Example you want to compare how different production machines look seen from the same point in space.

The attached Ilogic External Rule will copy the camera position and extents from the currently active document to all other opened documents. Camera position meaning your point of view in the active Inventor view.

Simply open all the Parts or assemblies you would like to compare and orient the active component correctly.

Activate Ilogic in your browser, switch to tab external rule, right click and add the attached rule below at the end of this post.

 When running :

• you have the option to use the same Zoom settings (called camera extents), or apply the same Zoom ratio compared to Zoom fit.
  Zoom ratio is useful in case your parts have very different sizes.

• You have the option to save the reoriented views as JPEG 1400*825 in the “C:\Temp” folder. When creating the pictures, we will switch off the 3D Indicator and switch it on again afterwards.

When an unlocked design view is active in any document, we enable the 2014 “Camera Autosave” Option so when switching Design View, it will save the camera settings.

Any comment let us know. Pierre Masson.

Download Copy_Camera_to_open_documents

 

VBA setting reflectivity and self-illumination in appearances

At the end of this post, you can find a VBA Macro that will scan a custom library and set Reflectivity and self-illumination to all the generic Appearances.

In Inventor 2014, the API fully supports Materials and appearances. Use this as a starting sample.

If you migrated your appearance library using the environment variable "InvCM_ForceConvertToGeneric" (see this article ).  Your custom colors belong to generic category, they do not have reflections and look a bit darker. This code will help.

• Rename the file extension in .BAS.
• Go to VBA Editor, import and import this file.
• Change the name of the library to treat. Ensure the library is loaded and not Read-Only in appearance editor. 
• Optionally remove comment signs to set generic color RGB Values to higher values.
• Change the values of reflectivity or self-illumination if needed.
• Run the code.

 

In the code you need you will find some comments to locate where you need to input your settings. The code is only processing materials from generic category, it will ignore the others.

For self-illumination, it will take the 10 % of the RGB Value of generic color. You can change these values in the code. Pay attention to self-illumination if you’re rendering your design in Showcase. You might end-up with undesired shadows.

 

Download Appearancelibrary

Pierre Masson.

 

Installing Office 365 will remove a local copy of VBA 7 module and prevents Inventor 2014 from working properly

If you cannot work properly in Inventor 2014 after having installed Office 365, follow the steps described in the solution below for solving the problem.

http://usa.autodesk.com/getdoc/id=TS21910314

Macros or VBA editor command button will not work in Inventor 2014 after installed from Suite installer

If you have installed Inventor 2014 from a Suite and VBA does not work, follow the steps described in the solution below for solving the problem.

http://usa.autodesk.com/getdoc/id=TS21623268

Adding Scale to Title Block

Sometime ago we have published the post below that allows to add the scale value from the first view on the sheet and put it in the title block, using an iLogic rule.

http://beinginventive.typepad.com/being-inventive/2011/06/base-view-scale-in-title-block.html

We have appreciated all the positive feedbacks received about the post, but also the concerns you have sent us about some limitations of the proposed solution.

The main one is that you have to create one different title block for each sheet, and, especially if you need to delete and add sheets to your drawings or templates, this is not practical.

So, the new solution proposed below doesn’t require the creation of a new iproperty to be added to a new title block for each sheet.

This is a simpler method that uses Prompted Entry text in the title block instead of an iProperty. 

In order to apply the new solution, do the following.

• Edit your title block definition and add a Text item with the type Prompted Entry

• This text should contain <Scale>

After you add this, Inventor will prompt you for a Scale value whenever you add the title block to a sheet.

The same happens when you add a new sheet with the title block to the drawing or when you start a new drawing using a template where you have applied this solution.

• When it prompts you, just leave the value blank

• Then add this Rule to the drawing

• Add the rule to the trigger “Before Save Document”

After that, on every sheet in the drawing, you will get the scale value from the first view on that sheet in the title block when you save the file.

Special thanks to Mike Deck for suggesting this new solution.

Ale

Update automatically drawing properties from model iProperties

You have copied some model iProperties in the drawing file of the model, following for instance the steps described in this article.

Of course you want to keep the model and drawing properties in sync, but you want to do that automatically, without having to remember to hit the “Update Copied Properties” button in the drawing.

In order to do that, you need to follow the steps below in the drawing.

• Menu Manage > iLogic > Add Rule.

• Create a rule using the Script you can download here.

• Menu Manage > iLogic > Event Triggers.

• Set the rule to run on the After Open Document and/or Before Save Document events or other events you may find more appropriate.

If you want, you can apply the steps above in a new drawing and save it as template.

Ale

Control Sketched Symbol and Title Block via drawing parameters using Ilogic

In your drawing, you want to control the geometry of your title block or sketch symbols. Unfortunately drawing parameters are not directly linked with Symbol or Title blocks dimensions.

We created a short Ilogic code to help you realize this.

You will have to create User Parameters like this :

“SymbolorTitleBlockname”_”Dimensionname”

For example : I am editing the Symbol named Rectangle and I want to control its parameter d3. I will a user parameter named “Rectangle_d3”

The same applies for Title Blocks. The rule is case sensitive.

 

The Ilogic rule inside the drawing will scan all your parameters. If it detects a parameter with an underscore :

• it will look for a Title Block or a Sketched Symbol with the same name
• it will change the dimension in the parameter name if it exists.
• it will do a check to ensure the Block or Symbol is still editable after change.

 

The file ParameterDrawing contains the Ilogic rule and some sketched symbols with the corresponding parameters so you can get familier with this Rule. You can download it at the end of the article.

Pay attention to the units, we are not checking the parameter units are corresponding to the sketch units. Concerning Event trigger, there is no Event option for Parameter change. One solution is to use the “Before Save Document” trigger.

Thanks to Brian Ekins and Mike Deck for the great tips.

Pierre Masson.

Download ParameterDrawing

Download CodeAsText

Major upgrade to the iLogic Code Injector tool

iLogic users of the world, rejoice.
Due to popular demand and with some help of my favorite Inventor developer, I made a major upgrade to the Code Injector tool.

Here are the improvements.

1. Filtering out AutoCAD dwg from the file selection
2. File selection searches also subfolders (but skips the OldVersions folders)
3. Improved the logic to detect an existing Inventor session.
   The tool makes the Inventor session invisible while the tool runs. Inventor becomes visible when exiting the tool.
4. Delete all rules and triggers in a series of Inventor files (via the "Delete all rules" button), defeating the original name of the tool as it now effectively can be used as a Code Rejector tool  or Code Removal tool :-)
5. Allow the selection of an existing rule from within an Inventor file (previously you either had to provide the rule text via copy and paste or by browsing to an existing text file).
   The new functionality can be accessed via the "Import from Inventor file" button.
   

As was the case before the changes, the tool will run on Inventor 2011 or later.

Hope you like the changes.
Bob

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