Ilogic and excell

[MrAcam04]

I created a parameter name called Material (multi line) and an excell file called Material as well. (A1=Nest-Pine A2=Nest-Oak A3=Nest-Maple). I need help on the ilogic end in order to have the parameter read the list in excell. I linked the excell file to my part file as well. Looking for help, thank you

[MjDeck · Accepted solution]

Here's a rule statement that should do it:

MultiValue.List("Material") = GoExcel.CellValues("3rd Party:filename.xls", "Sheet1", "A1", "")

This will read down the column until it finds a blank cell.

If you want it to read only up to a particular cell (such as A3), use this instead:

MultiValue.List("Material") = GoExcel.CellValues("3rd Party:filename.xls", "Sheet1", "A1", "A3")

This is looking on Sheet1.  Change the filename and sheet name if necessary.

(In the iLogic rule editor, this is in the System Snippets under Excel Data Links -> MultiValue list from Excel).

[MrAcam04]

Thank you very much

[MrAcam04]

Would it be possible to have the parameter Material & Color read staight from my styles Material & Colors?

[MjDeck]

This is not available for colors (but you could do it with the API).

For materials, here's a snippet:

MultiValue.List("Material") = iProperties.Materials

This is on the System Snippets, under iProperties -> List of Materials

It gives you all materials, so it's probably too much for any given part.

[MrAcam04]

Is it possible to pull the list of colors from the xml file? I tried this but it doesn't work

MultiValue.List("Color") = iLogicVb.Automation.ParametersXmlLoad(ThisDoc.Document, “G:\Design\Design Data\Colors.xml")

[MrAcam04]

In Ilogic under iproperties there is PartColor, is there a snippet that will allow me parameter field read the color iproperty. I tried the one below and received errors.

MultiValue.List("Color") = iProperties.PartColor

InventorVb.DocumentUpdate()

[MjDeck]

This is pretty easy using the API.  Here's how to do it:

 Dim colors as New ArrayList
 For Each renderStyle As RenderStyle In ThisDoc.Document.RenderStyles
   colors.Add(renderStyle.Name)
 Next

 MultiValue.List("Color") = colors
 

[MrAcam04]

Ok, Thank you very much for your time

I am not familiar with API but I am ready and willing to learn.

[MrAcam04]

This looks like a great place to begin learning. Thought I would help others find the information as well. Good Luck to you all

http://modthemachine.typepad.com/my_weblog/begging-api/

http://www.caddigest.com/subjects/adsk_inventor/tutorials.htm

Autodesk Inventor API

Part 1-3

[MrAcam04]

Where do I input this code you provided?

[MjDeck]

The code I provided:

Dim colors as New ArrayList
 For Each renderStyle As RenderStyle In ThisDoc.Document.RenderStyles
   colors.Add(renderStyle.Name)
 Next

 MultiValue.List("Color") = colors

can be used as an iLogic rule by itself.  Add a new rule in a part and paste in this code.

[MrAcam04]

NICE!

That worked like a charm, thank you very much for all your help.

[MrAcam04]

The parameter field filled in nicely, however when I pick a different color the part doesn't change with it. Would you know Why?

[MjDeck]

You have to add another rule to hook up the Color parameter.  Add a rule with just this line:

iProperties.PartColor = Color

[MrAcam04]

Looks good, thanks again

I was receiving errors because I was entering all the codes under one rule.