show appearances in part list

[Mike686]

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?

[Cadmanto]

See if this link helps you.

http://forums.autodesk.com/t5/Autodesk-Inventor/Export-BOM-parts-list-with-thumbnail-image/td-p/2662...

[Nicolas.Bourquin]

Hi,

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:

Step 1:

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")

Try

     prop = customPropertySet.Item("Appearance")

Catch

     customPropertySet.Add("", "Appearance")

End Try

iProperties.Value("Custom", "Appearance") =  iProperties.PartColor

Step 2:

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.

Step3 :

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.

Please, mark any response clicking on "Accept as Solution" button if it answers your question 

[Mike686]

thanks nicolas

i will try your method

and i will give you news if this works for me

[mtofts]

I have just tried this, and it uses the appearance from the material, and not from the title. I got 'Semi-polished'which is the finish of the material, but the title was called actually 'Dull polish'.

[Curtis_Waguespack]

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@mtofts wrote:
I have just tried this, and it uses the appearance from the material...

---

Hi mtofts,

This gets the active appearance name"

oColor = ThisDoc.Document.ActiveAppearance.DisplayName
MessageBox.Show(oColor, "iLogic")

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com