color style

[Anonymous]

hi,

is there a way where i can extract the color style of the material i choose for the part.ipt to be mapped out and show it in the title block?

inventor 2011

vault pro 2011

[bobvdd]

Several things need to be done to make this work.

Step 1:

Add the following iLogic rule to your part template file (or to existing part documents). It will create a custom property called "Colorstyle".

Trigger the rule "Before Save Document". This is important to make sure that the color in the custom property stays up-to-date every time the part gets saved.

customPropertySet = ThisDoc.Document.PropertySets.Item("Inventor User Defined Properties")
Try
     prop = customPropertySet.Item("Colorstyle")
Catch
     customPropertySet.Add("", "Colorstyle")
End Try
iProperties.Value("Custom", "Colorstyle") =  ThisDoc.Document.ComponentDefinition.Material.RenderStyle.Name

Step 2:

Start a new drawing. Go to the Document settings  and on the Drawing tab, use the "Additional Custom Model iProperty source" option to select the "Colorstyle" custom property from the ipt file prepared in Step 1.

Step3 :

Include the custom property "Colorstyle" in any text of your title block.

"Save Copy As" Template of the drawing  so that you don't have to repeat any of this for the next drawing 🙂

Cheers

Bob