Save drawing/part and then have to save again when closing???

[phlyx]

Been noticing this and kind of a time killer working on a simple drawing of a simple part.  Click the Save button at the top of the menu bar, set everything to YES, click OK and do it again.  So basically saved it twice.  The very next mouse click is closing the drawing and I get prompted saying there have been modifications to the files and asking if I want to save the files.  When I say YES it shows me both the drawing and the part require saving.  Why the heck do I need to save immediately after I saved without doing a single thing???

This is a link to the SWF capture file but can't find a good clean way to convert this to a playable video file:
https://drive.google.com/open?id=1m0jdNmf6bZYa5JYkoV03g4HRVZ077duz

[mcgyvr]

Yes there are times when Inventor seems to ask you to save again despite just having saved the file.. Supposedly they are trying to address some of those issues in regards to why files are marked "dirty" or "smudged" by Inventor and the users are confused as they haven't done anything as far as we know. 

In the future you may want to give Screencast a try for recording events in Inventor..

https://knowledge.autodesk.com/community/screencast

[Mark.Lancaster]

@phlyx 

For a given file it you want to see why its asking for it to be saved.

Select Help/About Inventor and when the Inventor about screen comes up, perform a CTRL+D

[phlyx]

Had a drawing open, did a Save, set everything to Yes and saved everything.  Then went to Help and About Inventor, then CTRL+D and got the popup below. 

Yet when I try to close the file it tells me both the drawing and the part needed saving:

Confusing.... 

[johnsonshiue]

Hi Scott,

If possible, please send the files to me directly (johnson.shiue@autodesk.com). There should be a logical reason to explain the behavior. Or, there is a bug. One thing you may want to look into is the iLogic rule. It may inadvertently dirty the file.

Many thanks!

[phlyx]

Doubt the file makes a difference as another engineer accessed the same files in the same project and didn't get the same results.  When I open a drawing (any drawing) and click Save, even if I just opened the drawing I get a prompt to save and it shows No on the drawing and Yes on the model.  Right after that if I click the X to close the drawing I get a prompt to save and both the drawing and the model are set to Yes.

When another engineer opens the drawing and clicks Save they get no prompt at all.  When the hit the X the drawing just closes.  We're running the same config files from the same location and the same project file.   We also have basically the same add-ins loaded.

No clue what is going on but starting to think I need to totally uninstall Inventor, erase everything related to it and do a clean install.  Too many haunted aspects of this.

[phlyx]

Found something that stopped this action.  Just testing around and when I set Application Options/Save/Embed Translation Report in Document to Do not create translation report my workstation functions properly.  When I click save on a drawing I just opened it doesn't prompt me for anything.  When I click the X it just closes the drawing with no prompt. 

Seems all fixed BUT (and there always seems to be a but) the engineer who was testing the same drawings as I was access has his set to Embed Translation Report in Document and he doesn't get the prompts.

[phlyx]

Getting back to this today.  I have a part open, I clicked on the Save button (no prompts, just saved it).  Then Did About Inv/CTRL+D and got the message below that Property Edit had changed.  Seems that Save wasn't saving that.

I shut down iPropWizard6 just to see as this had caused some other flaky things, and still got the same thing after doing a save.  Not sure what would be dirtying that property but that may also be why we're getting the prompt to save in a drawing even though Inventor says the drawing isn't dirty, might be the part the drawing references is dirty.  Any idea what could cause this property to be doing that?

[johnsonshiue]

Hi Scott,

Please send me the file (johnson.shiue@autodesk.com). Is there an iLogic rule running?

Many thanks!

[phlyx]

It's not file specific but I just tried some things to see if I could nail it down a little more.  I went back to the project and parts I was getting that dirty state with and now it wasn't doing it.  I could click Save, click X and it closed.  Then I made a minor change to the iProperties, clicked Save, then clicked the X immediately after and then I got prompted to save the file again.

If I save again, close it, re-open it and just click the X I get the same prompt.  If I open an assembly or a drawing that part is in, the assembly and the drawing does the same thing when I try to exit that file.   Also if I open a part and edit the part without changing the iProperties then I get a different prompt but forces me to do a second save right after saving it.

And once a file gets changed in any way, if you have an assembly or drawing open that has that component in it, it stays dirty regardless of how many times you save it or close it.   Once you save or close the assembly and/or drawing so no instances of that file are open, then it's like it resets itself and everything is good again.

Not sure how to check if any iLogic is running in the background.  And this does this same stuff regardless of iPropWiz being loaded or not.  Just in case you were wondering.

[johnsonshiue · Accepted solution]

Hi Scott,

Did you change iProperties via File Explorer? Or, you change it from right-click context menu in Inventor browser? The quickest thing to check if iLogic rule is running is to simply disable iLogic Add-In. Then try the workflow you did to see if the file gets dirtied.

Many thanks!

[phlyx]

Hey Johnson,

Nailed it!!!  I found a part and changed some iProperty a little, saved, closed and got prompted.  Did it but didn't change iProperty and it closed.  Repeated to be sure it was the same every time.  Set iLogic to not load automatically and had to restart Inventor (guess it can't unload while running).  Opened the same part and did it again and no matter what I did to iProperties when I clicked the "X" it just closed.  Looks like the guilty party is us.  I'll dig into that and post whatever I find out.

Thanks!!! 

[liam.dewhurstNMKYG]

Hey Team,

I'm getting the same problem, but we run an autosave pdf iLogic code (picked up from a forum).

Is anyone here smarter than me, and knows which line I might be able to change so that I get the pdf that I'm after, but the part isn't changed?

The save dialogue says that I've made user edits to the part (when it hasn't actually been touched)

'Export current drawing as a multi-sheet PDF
oPath = "S:\Production\Public Folders\PDF\"
oFileName = ThisDoc.FileName(False) 'without extension
oPDFAddIn = ThisApplication.ApplicationAddIns.ItemById ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}")
oDocument = ThisApplication.ActiveDocument
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium

oOptions.Value("All_Color_AS_Black") = 0
oOptions.Value("Remove_Line_Weights") = 1
oOptions.Value("Vector_Resolution") = 300
oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets
'oOptions.Value("Custom_Begin_Sheet") = 3
'oOptions.Value("Custom_End_Sheet") = 7

'get PDF target folder path
'Uncomment the following line to append \PDF onto the end of the current IDW folder location
'oFolder = Left(oPath, InStrRev(oPath, "\")) & "PDF"
oFolder = oPath

'Check for the PDF folder and create it if it does not exist
'If Not System.IO.Directory.Exists(oFolder) Then
'System.IO.Directory.CreateDirectory(oFolder)
'End If

'Set the PDF target file name
'oDataMedium.FileName = oFolder & "\" & oFileName & " Rev" & oRevNum & ".pdf"
oDataMedium.FileName = oFolder & oFileName & ".pdf"

'Publish document
oPDFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium)

MessageBox.Show("PDF saved", "File Save")

[johnsonshiue]

Hi Liam,

The behavior does not sound right. When exporting, the part and the drawing files should not need to be saved, unless there is unsaved change. Please share a simple example (idw, ipt) here. I would like to understand the behavior better.

Many thanks!

[liam.dewhurstNMKYG]

Hey Johnson,

I think I figured out why it's happening.

It's our upRev automation, where if you change the rev of the drawing it changes the rev of the part. (our factory references the rev of the part & rev of drawing)

However this automatically pushes the rev back to the part every time we save (iTrigger). So anytime we save it changes iProperties (frustrating). Is there a way to do a checksum with an if/else loop so that we check if the drawing and part match rev, and only push the ipropoerty change if they don't match?

Dim odrawdoc As DrawingDocument
odrawdoc = ThisDrawing.Document
Dim odoc As Document
Try
odoc = ThisDrawing.ModelDocument
odoc.PropertySets.Item("Summary Information").Item("Revision Number").Value = odrawdoc.PropertySets.Item("Summary Information").Item("Revision Number").Value
Catch
End Try

[bshbsh]

if odoc.PropertySets.Item("Summary Information").Item("Revision Number").Value <> odrawdoc.PropertySets.Item("Summary Information").Item("Revision Number").Value then
odoc.PropertySets.Item("Summary Information").Item("Revision Number").Value = odrawdoc.PropertySets.Item("Summary Information").Item("Revision Number").Value
end if

[liam.dewhurstNMKYG]

Hi Bshbsh,

This worked like a charm, thanks!

Dim odrawdoc As DrawingDocument
Dim odoc As Document
odrawdoc = ThisDrawing.Document
odoc = ThisDrawing.ModelDocument

If odoc.PropertySets.Item("Summary Information").Item("Revision Number").Value <> odrawdoc.PropertySets.Item("Summary Information").Item("Revision Number").Value Then
odoc.PropertySets.Item("Summary Information").Item("Revision Number").Value = odrawdoc.PropertySets.Item("Summary Information").Item("Revision Number").Value
End If

[Matthew_Policelli]

We often have this problem come up on our files, and what solved it for the OP doesn't seem to help us.

In one instance, I checked the save status and it says non-shape edit. What does that even mean? It's agonizing when Inventor asks me to check something back out again right after I checked it in.

[johnsonshiue]

Hi Matthew,

If I understand the dirty flag correctly, this is probably related to property edit. Is it possible, there was some change in the iProperties made outside of Inventor requiring Inventor to update the file?

Please share an example that exhibits the behavior. It could be a bug. Or, there is some corruption in the file leading to excessive file-dirtying events.

Many thanks!