Hi, i'm trying to show the appearance of the part in a part list next to the column material
and i can't find how to do it
can someone help me?
See if this link helps you.
Here is a possible solution using an “illogic” rule you could use in a BOM of an idw file to show the "value" of the "appearance" of the model.
But several things need to be done to make this work:
Add the following iLogic rule on every existing parts file (or directly into the template if necessary).
It will create a custom property called "Appearance" and will copy the value of the "Appearance" of the ipt file.
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")
prop = customPropertySet.Item("Appearance")
iProperties.Value("Custom", "Appearance") = iProperties.PartColor
Go in the assembly (iam) and edit BOM>Add iProperties column> create a new column >write Appearance>ok
To verify Edit “BOM” and verify the column “Appearance” is visible > Save the template.
Start a new drawing. Go to the “Document Settings” > “Drawing tab” > "Additional Custom Model iProperty source" to select the ipt file prepared in Step 1 > “Copy Model iProperties Settings” to select the “Appearance”.
Place a view of the Assembly prepared in step 2 and insert a BOM
Edit BOM > Column Chooser > New Properties > select “Appearance” > ok
=> A new column should be visible with the Appearance value of the different components..
Remark: You could have also the possibility to include all these manipulations directly in your templates.
I hope this will help you.
Access a broad range of knowledge to help get the most out of your products and services.
Download & InstallationGetting your Software
Subscription ManagementSign In / Create Account