- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hello.
I would ask for information if Inventor 2015 is able to automatically assign names of Sheets in the * idw file as one of the iProperties parameters from the 3d model of the * .iam or * .ipt file?
I will be grateful for any help.
Sincerely
Wojciech Janko
Solved! Go to Solution.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Yes you can... Can you please give an example of what you're trying to do so we can give you a relevant example
Mass Override for Each Model State
Custom Glyph Icon for iMates
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hello.
I would need to automatically name Sheets.
I have a * .idw document file, which has about 100 sheets, on each sheet there will be a single part (* .ipt) or assembly (* .iam).
I would like the name of the sheet to be automatically changed from "Sheet" to the string which was entered in iProperties -> "Project" -> "Version number".
for examples: "Sheet" -> "2.1.1.3.5"
I would be extremely grateful for your help, because manually naming each sheet is quite laborious and you can be mistaken.
Greetings.
Wojtek
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
It would look something like this.
Dim app As Application = ThisApplication
Dim doc As DrawingDocument = app.ActiveDocument
Dim oSheet As Sheet
Dim oView As DrawingView
Dim docM As Document
For Each oSheet In doc.Sheets
oView = oSheet.DrawingViews(1)
docM = oView.ReferencedDocumentDescriptor.ReferencedDocument
oSheet.Name = docM.PropertySets.Item("Design Tracking Properties").Item("Part Property Revision Id").Value 'I couldn't find "Version Number" in "Project" but I'm in 2018
'oSheet.Name = docM.PropertySets.Item("User Defined Properties").Item("Version Number").Value 'This would be for a custom property
Next
Mass Override for Each Model State
Custom Glyph Icon for iMates
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hello.
Thank you for the program, but it does not end up changing the name to "Revision Number".
In the drawing I have marked what needs to be copied and where to insert.
I just wanted to point out that "iProperties" are from the 3D model and the sheet name is in the * .idw document file.
I would be grateful for your help in solving this problem.
Sincerely
Wojtek
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Try this for Revision Number...
Dim app As Application = ThisApplication Dim doc As DrawingDocument = app.ActiveDocument Dim oSheet As Sheet Dim oView As DrawingView Dim docM As Document For Each oSheet In doc.Sheets oView = oSheet.DrawingViews(1) docM = oView.ReferencedDocumentDescriptor.ReferencedDocument oSheet.Name = "words to prepend here" & docM.PropertySets.Item("Inventor Summary Information").Item("Revision Number").Value & "words to apend here" Next
Sorry I don't see a marked up drawing... screen shots might help me understand what you want better. I was under the impression you would want the iProperty from the model because it went with the only part on that sheet.
Mass Override for Each Model State
Custom Glyph Icon for iMates
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hello.
Thank you very much for your help, the formula works perfectly ![]()
You are great ![]()
Thank you again and best regards ![]()