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Export Parameters as iProperties

I recently made a mistake.  While working on a project, I should have marked some User Parameters to Export as iProperty.  Unfortunately, I didn't realize this until I was about 300 parts in.  I sure didn't want to open up each part and manually check those boxes.

For those unsure of what I'm referring to, in Inventor you can export Parameters as iProperties.  This is a very easy and simple way of getting model data onto your Bill Of Materials or Parts Lists.  You accomplish this by checking the box in the Export Parameter column of the Parameters dialog box.

Once you've marked one or more parameters to Export, you can right mouse click on one of the marked Parameters and choose Custom Property Format from the Contextual Menu.

  From there, you can format the iProperty to suit your needs.

As I mentioned, I sure wasn't going to open each part and export the necessary Parameters and set their format.  Automation to the rescue!

The Inventor Parameter API object has a Property called ExposedAsProperty.  This is set to a Boolean that controls whether or not the parameter is exposed as an iProperty.  Assuming I've already declared and set the oUserParam object:

oUserParam.ExposedAsProperty = True

Once that property has been set to True, you can set all the options for the formatting thru the Property called CustomPropertyFormat.  

oUserParam.CustomPropertyFormat.PropertyType = kTextPropertyType
oUserParam.CustomPropertyFormat.Precision = kThreeDecimalPlacesPrecision
oUserParam.CustomPropertyFormat.ShowLeadingZeros = False
oUserParam.CustomPropertyFormat.ShowTrailingZeros = True
oUserParam.CustomPropertyFormat.ShowUnitsString = True
oUserParam.CustomPropertyFormat.Units = "in"

The PropertyType Property determines if the iProperty will be a Number or a Text Property.  It uses the CustomPropertyTypeEnum.

The Precision Property determines the precision of the iProperty.  It uses the CustomPropertyPrecisionEnum.

The ShowLeadingZeros and ShowTrailing Zeros determine if leading or trailing zeros are included in the iProperty.  These are set to Booleans.

The ShowUnitsString Property determines if the unit string is shown in the iProperty.

The Units Property determines the units to use in the iProperty.

You can look up the enumerators in the Inventor Programming/API Help for more information on them. 

In my case, I had three specific Parameters (Height, Length, Width) in each part that I wanted to expose.  Admittedly, there are many ways I could have done this.  I chose to loop thru all the User Parameters and if the Parameter name matched what I wanted, I exported it and set its format to the way I needed it.

Below is the final code:

Imports Inventor.CustomPropertyPrecisionEnum
Imports Inventor.CustomPropertyTypeEnum

' Declarations
Dim oPart As PartDocument
oPart = ThisApplication.ActiveDocument

Dim oCompDef As PartComponentDefinition
oCompDef = oPart.ComponentDefinition

Dim oUserParams As UserParameters
oUserParams = oCompDef.Parameters.UserParameters

' Loop thru parameters and set specific parameters to export as iProperty
For i = 1 to oUserParams.Count
    sName = oUserParams.Item(i).Name
    Select Case sName
        Case "Height", "Length", "Width"
            oUserParams.Item(i).ExposedAsProperty = True
            oUserParams.Item(i).CustomPropertyFormat.PropertyType = kTextPropertyType
            oUserParams.Item(i).CustomPropertyFormat.Precision = kThreeDecimalPlacesPrecision
            oUserParams.Item(i).CustomPropertyFormat.ShowLeadingZeros = False
            oUserParams.Item(i).CustomPropertyFormat.ShowTrailingZeros = True
            oUserParams.Item(i).CustomPropertyFormat.ShowUnitsString = True
            oUserParams.Item(i).CustomPropertyFormat.Units = "in"
    End Select
Next I

I ran this code as an external rule.  I used a custom application that I wrote that allows me to run rules against a large group of parts.  I accomplished in a few minutes what would have taken me hours to do....and I know it's all correct!

If you have any questions, be sure to post in the comments below.

Happy Coding!

Randy

 

Inventor 2019.1 Update: iLogic Log

The latest update for Autodesk Inventor gave us the iLogic Log.  If you either write iLogic rules or have to debug iLogic rules, it's worth your time to continue reading and check out this new tool.  It really goes without saying that if you do the former, then you're going to be doing the latter as well.  Also, if you've always wanted to be a logger, then continue on!

Logger Function

The iLogic Log gives you a better understanding of what is going on while your iLogic rules are running.  Have you ever needed to know what value a variable had at a particular point or wanted to know which block you were getting into inside of a conditional statement?  The Log will let you to do that in an easy manner.  Previously you may have thrown this type of information out to a message box that had to be acknowledged before the rule would continue.

The iLogic Log allows you to print data in the Log panel by using the new Logger function.  The context for the function is Logger.LogLevel("your message").  There are multiple levels that you can use in the LogLevel placeholder.  They are (in order): Trace, Debug, Info, Warn, Error, Fatal, and None.  The active Log Level determines what log message get printed to the Log.  Only those functions that use a level at or below the active Log Level will be displayed.

For example:  I would like to know the value of the Overall_Length parameter at a certain point in one of my rules.  My active Log Level is Info.  This means I'll see any Logger functions that use Info, Warn, Error, or Fatal. 

I've created a rule in my part called Initial_Rule.  I've entered the following lines into this iLogic rule:

Logger.Info("Overall_Length: " & Overall_Length)

iLogicVb.RunRule("Secondary_Rule")

When the rule runs, I'll see the following:

INFO|Overall_Length: 86.625

To turn on the Logger panel, either use the Show Tabs icon on the Model Browser or the User Interface flyout in the Windows Panel of the View Tab of the Ribbon.

 

You can set your active Log Level through the Advanced iLogic Configuration dialog box.  You can also select the active Log Level through a drop down that appears when you first open the iLogic Log Panel but I have yet to figure out how to get that menu back! 

Trace Function

You can also use the new iLogic Log to trace when your rules fire.  Setting the active Log Level to Trace will cause the Log panel to also show when you are entering and exiting a rule.

In my example scenario, I've created an additional rule called Secondary_Rule and entered the following lines into it:

Logger.Info("Secondary Rule ran")

When I run the Initial_Rule, I get the following ouput in the Log panel:

INFO| 1: >>---------------------------
TRACE|Entering rule: Initial_Rule (in iLogic Logger.ipt)
            INFO|Overall_Length: 86.625
            TRACE|Entering rule: Secondary_Rule (in iLogic Logger.ipt)
                        INFO|Secondary Rule ran
            TRACE|Exiting rule: Secondary_Rule (in iLogic Logger.ipt)
TRACE|Exiting rule: Initial_Rule (in iLogic Logger.ipt)

I've been using DebugView (download here) for years to accomplish this same thing.  If you're not on Inventor 2019.1, I'm afraid you won't be able to use the new iLogic Log.  In that case, I suggest looking into DebugView.  Click here to read an older blog post about DebugView.

Some of the benefits the iLogic Log has over DebugView:

• Internal to the program so there's no need to download something else
• No need to use a filter to limit what Logger sees as is needed in DebugView
• Built in Trace (although I always put lines at the front and back ends of my rules to emulate this)
• Log will capture your log data even if it isn't open when the rules run

Some of the benefits DebugView has over the iLogic Log:

• Can change the font size
• Can emphasis lines using the Highlight controls
• Can set the window to Always On Top

 

As with DebugView, there's really no need to remove the Logger function lines from your code.  You can adjust the active Log Level to something higher than the level you've specified in your code but I've found it just as easy to leave it all there and ignore what I don't want to see.  

I hope you can imagine how helpful this is!  If you have any questions, be sure to post in the comments below and as always, Happy Coding!

Randy

*** UPDATE 9-20-2018 ***

You can change the font size in the iLogic Log.  You can use CTRL+PLUS and CTRL+MINUS to zoom in and out after giving focus to the iLogic Log.  You can also use CTRL+F and a zoom indicator will show up at the bottom of the iLogic Log panel.  Big thanks to Mike Deck @ Autodesk for pointing that out!

Can I do that with the Inventor API?

Quite often I am faced with a challenge to control something new with code.  If you read my iLogic: Where do I go from here blog post, then you at least know a little about using the Help file to look up methods and properties for objects.

In that post I had you search for table in the Programming/API Help and then choose CustomTable Object from the search results.  I never gave you any additional help on how to choose that search term.  In the case of the General Table it was pretty straightforward.  But what if it's not?

The method shown in this post will help you understand what the API calls objects, which in turn will assist you in searching for it.

First, create the object in Inventor using the standard manual process.  In this example, I'll be looking at the General Table again so I've created a blank General Table in a drawing.

Next, fire up the ol' VBA Editor, create a new procedure, and enter the code below:

Public Sub TestObj()
    Dim obj As Object
    Set obj = ThisApplication.ActiveDocument.SelectSet(1)
End Sub

Now we have two different ways we can see the type of the object.  We can either set a breakpoint at the Set obj line and look at the Locals window or we can set a Watch on the obj expression.

I suggest turning on your Debug toolbar if you don't have it on already.

1. Run Sub
2. Reset
3. Toggle Breakpoint
4. Locals Window
5. Watch Window

To set a breakpoint:

Ensure your Locals window is visible in the VBA Editor.  If it is not visible use the Locals Window button on the Debug toolbar to turn it on.

Place your cursor anywhere in the End Sub line and select the Toggle Breakpoint tool on the Debug toolbar.  You'll see a red dot in the left column of the Editor window.  You can also click this area to toggle a breakpoint.  Once the rule gets to this line, it will break and allow you to control when and how it moves forward.  We are setting it here on the End Sub so that the obj object will already be set.

To set a watch:

Ensure your Watch window is visible in the VBA Editor.  If it is not visible use the Watch Window button on the Debug toolbar to turn it on.

Select the obj text in the procedure.  Right mouse click and choose Add Watch... from the contextual menu.  I'd suggest changing the Watch Type to Break When Value Changes.  This will break the code when the value for obj changes.

Back in Inventor, select the entity that you created (the General Table in my case) and then run the TestObj procedure by clicking on the Run Sub button on the Debug toolbar.

If you've set a breakpoint, then the rule will break at the End Sub line.  Take a look at the Locals window, find the obj object, and look in the Type column.  In my case where I selected the General Table, I see Object/CustomTable. 

If you've set a watch, you'll need to look at the Watches window.  The expression that you are watching should show up along with it's Value and Type.  In my case where I selected the General Table, I see Object/CustomTable.

Now I know the API considers this a CustomTable so I can go to my Programming/API Help, search for CustomTable, and read all about it.  Be sure to stop your code by clicking the Reset button on the Debug toolbar!

In addition, you can also use this method to determine if something can be controlled by code or if it is supported by the API.  If the Type is just Object or Empty or if you see Nothing or <Out of context> in the Value column, that means that type of object is not supported by the API at this time.

Thanks and Happy Coding!

Randy

Named Entities & Attributes in Inventor 2019

A few of my favorite new features in / additions to Inventor 2019 is the Assign Name command and using those assigned names in Constraints.

I’ve been using attributes for many years in order to “get” geometry that’s required, whether it be for the purposes of constraining, adding annotations to drawings, or just finding a specific feature. 

The Assign Names command creates attribute sets and attributes with specific names.  The AttributeSet is named “iLogicEntityNameSet” and the attribute is named “iLogicEntityName” with the value being whatever you name the entity.  See example below:

 

I was curious how attributes that were created either programmatically or with AttributeHelper would interact with the new functions.

A few things to notice about attributes that are created either programmatically or with AttributeHelper:

·         If named properly (see above), these attributes will show up in the graphics window (you may have to hide and unhide labels)

·         By default, these attributes will not show in the Geometry Tab of the iLogic Browser Panel.  If you rename it by using the right mouse click Edit Name, it will show in the Geometry Tab.

Attributes that are created either programmatically or with AttributeHelper can be used in the new 2019 Relationships (Add) snippets, as long as they are named as per above.

Thanks and Happy Coding!

Randy

iLogic: Where do I go from here?

One question that I get quite often is “Where do I go to learn more advanced iLogic?”  My first response is do you know any programming?  If not, it would really help you advance your iLogic skills to know some basic programming concepts and skills.

One way to describe iLogic is that it is a user-friendly wrapper around the Inventor API (application program interface).  It allows you to easily change parameters, suppress features, move a drawing view, etc. without having to understand how the Inventor API works.

If you’re not familiar with Object Oriented Programming (OOP), I’d suggest that you read up on that to begin with.  There is some very good introductory information on OOP in the online Inventor API User’s Manual online help, which you can access here.  It discusses objects, explains their relationships, shows you the Object Model (shown below in very low res), and all kinds of other goodies.

For this post, let us assume that I have a need to move a table on an Inventor drawing.  I’m going to explain how I would go about figuring out how to do that (that whole teach a person to fish thing).  In case you missed it, my last blog post was about just that, moving a table.  You can read that post here.

For now, I’m going to assume that we are fairly versed in the API and know everything else in my Moving Custom Tables With Code post, other than how to move the table.  Don’t worry, we’ll revisit the rest in future posts.

I start off with the Inventor Programming/API Help.  You can access this by clicking the drop down next to the Help Question Mark icon on the right hand side of your Inventor title bar, hovering over the Help and then choosing Programming/API Help.

Go to the Search tab of the help and enter table. 

You’ll see a lot of results, things like CustomTable Object, HoleTable Object, RevisionTable Object, etc.  In this case, we want to choose CustomTable Object.  Admittedly, it’s not very straightforward to know that we want a CustomTable Object since the Inventor command is called General Table. 

Once you’ve clicked on the CustomTable Object, you’ll see the various methods and properties associated with that object.  You can think of methods as actions against an object and properties are data associated with that object.  Take a moment to look through the various options and then look at the Position property in particular.  Its description says “Specifies the position of the table”.  That’s what we want to set.  If you click on Position, we’ll see the help page associated with it.  It lists the following:

• Description: We’ve already seen this on the last page
  • Specifies the position of the table
• Syntax: How the property is to be used in your code
  • CustomTable.Position() As Point2d
• Property Value: This tells you that it’s a read/write value and it requires a Point2d, which is also given to us in the Syntax
  • This is a read/write property whose value is a Point2d
• Version: This tells us what version of the Inventor API this was introduced
  • Introduced in version 9

Based on this, I now know that I can move or set the position of my custom table by the following steps:

1. Get a reference to the table I want to move
2. Create a Point2d
3. Pass the Point2d to the Position property of my table

To make it easier, I’m going to post the code from my previous post below.

' Declarations. Assuming this is a drawing

Dim oDrawDoc As DrawingDocument

oDrawDoc = ThisApplication.ActiveDocument

' Assuming first sheet

Dim oSheet As Sheet

oSheet = oDrawDoc.Sheets(1)

' Assuming first custom table found

Dim oTable As CustomTable

oTable = oSheet.CustomTables.Item(1)

' Get height of table. Insert of table is at top of table.

' Height is required if you want to drive by bottom of table.

Dim oHeight As Double = oTable.RangeBox.MaxPoint.Y - oTable.RangeBox.MinPoint.Y

' Set point. Dimensions are in cm

Dim oMultiplier As Double = 2.54

Dim oPoint As Point2d

oPoint = ThisApplication.TransientGeometry.CreatePoint2d(1 * oMultiplier, 1 * oMultiplier + oHeight)

' Move table

oTable.Position = oPoint

I hope that I’ve shed a tiny bit of light on the Inventor API and how you can go about searching for what you need.  In future posts, I’ll dig a little deeper into the API.

Thanks and Happy Coding!

Randy

Moving Custom Tables With Code

I was recently asked if it's possible to move the position of a custom table on an Inventor Drawing using iLogic.  The straight answer to that question is "No".... but we can do it with a little API code.

Unfortunately, there are no out of the box iLogic Snippets that give us access to a custom table.  For this, we need to dig into the API just a bit.

The CustomTable object is accessed through the Sheet object, which is accessed through the DrawingDocument.  In the example code below, I'm assuming that the drawing we're working in only has 1 sheet and also that it only has 1 custom table.  I'm also not verifying that a custom table exists.  If you want to run such a rule against drawings that may not have a custom table, you'd want to check and exit the rule if there are none.

The position property of the CustomTable object is based on the upper left corner of the table, regardless of how the table layout is set up on your Styles & Standards.  Because of this, I'm also determining the height of the table so that I can position the table by it's lower left corner.  I'm doing this by subtracting the MinPoint.Y from the MaxPoint.Y.

Remember, values in the API are in centimeters.  I typically create a multiplier object and use that throughout my code.  In the example below, I'm positioning the lower left corner of my table 1" in the X and 1" in the Y from the drawings 0,0.

' Declarations. Assuming this is a drawing
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Assuming first sheet
Dim oSheet As Sheet
oSheet = oDrawDoc.Sheets(1)

' Assuming first custom table found
Dim oTable As CustomTable
oTable = oSheet.CustomTables.Item(1)

' Get height of table. Insert of table is at top of table.
' Height is required if you want to drive by bottom of table.
Dim oHeight As Double = oTable.RangeBox.MaxPoint.Y - oTable.RangeBox.MinPoint.Y

' Set point. Dimensions are in cm
Dim oMultiplier As Double = 2.54
Dim oPoint As Point2d
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(1 * oMultiplier, 1 * oMultiplier + oHeight)

' Move table
oTable.Position = oPoint

Let me know in the comments if you have any further questions or comments. 

Thanks and Happy Coding!

Randy

Share Your Best Product Design & Manufacturing Collection Tip for the Chance to Win $500

If you’re an Autodesk Product Design & Manufacturing Collection pro, it’s time to share your wisdom! The Product Design & Manufacturing Collection (PDMC) Skills Challenge has begun. To enter this video contest, submit a one-minute tip for using one of the products in the collection. Here’s an example of a YouTube quick tip created by Inventor Luke.

The first place entry will win $500, second place will win $300, third place will win $200, and the fourth through tenth place entries will win $100.

Ready to enter?! Here are the details:

• Download the latest version of the Autodesk product you want to use, if you haven’t installed it already.
• Record your tip in a 60 second video. If you need a recording tool, you can download Autodesk Screencast for free.
• Submit your video on IMAGINiT's Facebook, Twitter or LinkedIn page. Include the hashtag #MyPDMCTip in the description.
• Enter by October 11^th.

All entries will be judged by a panel of experts and the winner will be contacted via social media. Remember, you can submit more than one tip to share your expertise with the PDMC community!

Inventor Progress Bar

For a recent automation project, I had to run code against multiple parts in an assembly.  This group of parts could be a significant number.  At run-time, the client wanted to see an overview of how many files were to be processed for the current configuration and what number have already been processed.

I knew Inventor had a Progress Bar but up until recently, I had yet to have a good reason to use it.  

To use the Progress bar, you need to define the following:

• Progress Bar title:
  • I'm using "Creating DXDF Files..." in the code below
• Total count of files to be processed
  • I'm using the count of an array (sDXFOutList).  This portion has been removed from the code sample below.
• Current file being processed
  • This is an incremented value

Create the progress bar before you get into your loop and be sure to close it after the loop.  While in the loop, I'm incrementing the current file and updating the progess bar.

Below is the sample code and an image showing the Progress Bar during run-time.  I've removed portions of the code that doesn't directly reflect the Progress Bar portion of the code.

Replace the portion that says ' Your code with whatever you need to do to each component occurrence.

 

Sub Main()

    ' Additional code has been removed

    ' Setup Progress Bar
    Dim DXFOutCount As Integer = sDXFOutList.Count
    Dim oMessage As String = "Creating DXF files...."
    Dim oProgressBar As Inventor.ProgressBar
    oProgressBar = ThisApplication.CreateProgressBar(False,DXFOutCount,oMessage)
    Dim iDXFFile As Integer = 0
    

    ' Cycle through each occurrence
    For Each oCompOcc In oLeafOccs
        iDXFFile += 1

        ' Update the progress bar to reflect which part is being operated on
        oProgressBar.Message = ("Processing file " & iDXFFile & " of " & DXFOutCount & "...")
        oProgressBar.UpdateProgress

        ' Run Code Here
            ' Your code

    Next

    ' Close the progress bar
    oProgressBar.Close

End Sub

 

iLogic Rules Editor: Save Vs. Save & Run

Sometimes we want to make changes to our iLogic rules but we do not necessarily want the rule to run after making these changes.  In earlier releases of Inventor, the Rule Editor only has two buttons, OK and Cancel (see image below).

If you click OK, the rule will run immediately.  If you click Cancel, you would lose the changes you made to the rule.  Below are a few workarounds that can be used to save your changes in releases prior to 2017 and which one to use depends on your circumstances:

If you are okay with the rule running but you know that the rule will cause an error:

1. You can click OK and rule will run
2. When error pops up, accept the error
3. The IDE will pop open again
4. Click Cancel.  (Don’t worry, the changes you made will be saved)

If you do not want the rule to run immediately:

1. Go to the Options tab of the Rule Editor
2. Click the Suppressed check box (see image below)
3. Click OK
4. In the Rules tab of the iLogic Browser, right click on the rule and Unsuppress it.

As of Inventor 2017, there were changes made to the iLogic Rule Editor that make it a little easier to edit rules, specifically, we now have the Save button.

The Save button will save your rule and close the Rule Editor without running the rule.  The Save & Run button does what OK used to, closes the Rule Editor and runs the rule.

“Give a man a program, frustrate him for a day.  Teach a man to program, frustrate him for a lifetime.” - Waseem Latif

Randy