Being Inventive

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

Putting user parameters to work in part sketches in 2013

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

Creating an ellipse based on its focal points

It has been a while since I have blogged about sketches in Inventor and I thought the new Equation Curve command in Inventor 2013 would be a good occasion to diversify the topics covered on this blog, while at the same time highlighting a cool new feature.

A nice example I can think of is to experiment with ellipses. Inventor generates an ellipse starting from a center point and by defining the extents of the major and minor axis.

But how would you create an ellipse based on its two focal points and the minor axis? It all depends with what Inventor release you are working with.

In 2013:

You can now create an ellipse with two focal points with the new Equation Curve command by using an explicit polar equation. See this part file for an example.

The mathematical definition of such an ellipse based on its two focal points is

r = (B^2)/(A-C*cos(Q))   with Q between 0 and 360 deg

 

Fig 1: Ellipse with half focal distance C shown

A= half major axis

B = half minor axis

C= half the distance between the two focal points

r (radius) and Q(angle) being the polar coordinates of a point on the ellipse (radius and angle)

At the same time A, B and C have to respect the following equation:

A^2 = B^2 + C^2

I have chosen to implement this formula into the parameters dialog:

Fig 2: Parameters dialog takes care of relationship between A, B and C

Note: I added an index 1 to the parameters and used A1, B1 and C1 instead of A, B and C to avoid confusion with reserved parameter keywords.

The result of using such an equation curve can be seen below. The first focal point sits on the origin. To create the second focal point you could for instance mirror the first one along the minor axis.

Fig 3: Creating an ellipse via an explicit polar equation

In 2012 (or earlier versions):

There is not such a thing as equation curves in 2012 unfortunately. But you can quite easily create such an ellipse via the API in the older versions.

You can download here a sample VBA project that you can load in the VBA editor with the Load Project command.

To run the code, run the macro called ShowEllipseDialog

It creates an ellipse with one of its focal points positioned on the origin and the major axis aligned with the X-axis.

You need to have a XY sketch active before running the dialog. The two focal points are connected with a construction line.

B and C values can be freely chosen but A is automatically calculated based on the A^2 = B^2 + C^2 formula.

Fig 4: Creating an ellipse via the Inventor API

Bob

Injecting iLogic code and iLogic event triggers automatically

I have posted about a similar subject a while ago. The idea is to copy and paste an existing iLogic rule in a series of Inventor files.

In the solution that I offered originally I was able to accomplish this but there was a missing link.
What good would an iLogic rule be that was created in an automatic way when at the same time you cannot decide when the rule will run?
This kind of defeated the whole purpose of automatically adding AND running rules on certain events throughout multiple files.

One of the loyal readers of the blog came to the rescue.
Megajerk has graciously provided the source code and the executable for a VB.NET tool that completely automates the process. So I decided to post this tool on the Inventor support blog on behalf of him.
The tool is called "Code Injector" and can be downloaded from here.

After unzipping the tool to any location on your disk drive and when you start the file …\Code Injector\Code Injector\bin\Debug\Code Injector.exe, you will see following dialog:

Fig 1: Code Injector in action ( (click here to see a full size screenshot)

Note that I have selected two part files in the dialog, defined an iLogic rule that displays the name of the active document and the rule gets triggered on open.

From the way the buttons in the dialog are labeled you can easily figure out most of the other tool options:

• Open multiple files from the types ipt, iam and idw from a folder
• Either copy and paste the rule text or import it from an existing text file
• Overwrite rules with duplicate names or not
• Run rules on creation or not

Once the tool has finished , you will se an Operation complete dialog that you can dismiss.

One small quirk is that rules that get added and that are set to trigger before or after save, ignore the setting of the "Run rules on creation" checkbox.
Such rules will automatically run while the Inventor files get saved by the tool. It is a sort of chicken and egg thing which is difficult to avoid.
Rules that trigger on open obviously obey the checkbox. Thanks again to Megajerk for sharing his tool with all of us.

Bob

Extruding and Shelling all the closed loops in a sketch

In your part sketch you have a large quantity of closed loops.

(I.e.: You have imported in the Inventor part sketch a dxf or dwg generated from an external application.)

You want to extrude and subsequently shell all them in one go.

For doing that you can do the following:

• Download and unzip this VBA Macro to your local drive.
• Menu Tools > Options > VBA editor.
• Load the file ExtrudeShell.ivb via the File > Load project command in the VBA editor.
• Run the macro called PipeExtrusion.

• In the following Pipe shape dialog enter the Height and Wall thickness values.
  • The values need to be entered as digits without units nor formulas.
  • The input is in default length units as set in the Document settings.
  • Entering a positive wall thickness adds more material to the outside of the sketch curves, entering a negative wall thickness adds material to the inside.
• Click on the Select sketch button and select the sketch in the browser.

• Click OK and get the result.
  • If the result is not the one you want, click on Undo and repeat the steps entering the appropriate values.

Inventor File Reserve 2012

You want to convert legacy Shared or Semi-Isolated projects to Vault or Single User projects, but some of the files in the project are reserved / read-only.

The attached tool allows you, between other functionalities, to un-reserve in one go all the files of the project.

For using the tool, download FileReserveR2012 and extract the files on your machine.

Read very carefully the readme file before using the tool.

Rename the file FileReserveR2012.___ to FileReserveR2012.exe.

The tool works with all older Inventor versions (from R6 – R2012).

Below you can find more details about some of the functionalities provided by the tool described in the readme file as well.

• Remove or Apply reservation flags from Inventor files.

UserXY owns the files.

   

Context menu or File Menu will provide Check In / Out functionality.

• Remove or Apply reservations from different users.

All selected files can be processed in one go.

• Search for all files from project (*.ipt, *.ipn, *.idv, *.iam, *.idw / *.dwg)

• Indicate files which have been created with Student version.

True = Educational file

False = non educational file

Not available = File Reserve used with Inventor Release < 2010

The tool, of course, doesn’t change the Educational condition of the file.