Change between different JPG's in title block (using iLogic)
@Anonymous
I've got you covered:
https://knowledge.autodesk.com/community/screencast/62d50fd9-e36c-4f7e-b441-13bc3f8dce55
You can find 3 rules attached. Change them as you see fit.
If you want to make the form exactly the same:
This is a quickie code, but does the job for me in my tests. It looks in the 'active' sheet of the 'active' drawing for the first SketchImage, captures its 'position', deletes it, then adds another image at that same position.
I suppose you could do more to control the size and orientation of the other image, but if both images are the same type, size, orientation, resolution, etc, it most likely wouldn't cause any problems. You could also use the SketchImage's 'BoundaryGeometry' to help control it.
Anyways, here's the iLogic code:
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("A Drawing Document must be active for this rule to work. Exiting.",vbOKOnly+vbCritical, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisApplication.ActiveDocument
Dim oSheet As Inventor.Sheet = oDDoc.ActiveSheet
Dim oTBDef As TitleBlockDefinition = oSheet.TitleBlock.Definition
Dim oSketch As DrawingSketch
oTBDef.Edit(oSketch)
Dim oImg As SketchImage = oSketch.SketchImages.Item(1)
Dim oPos As Point2d = oImg.Position
oImg.Delete
oSketch.SketchImages.Add("C:\Temp\Replacement Image.png", oPos, True)
oTBDef.ExitEdit(True)
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Wesley Crihfield
(Not an Autodesk Employee)
If you're used to coding in vb.net, that's great, because iLogic uses vb.net. In Inventor, iLogic is an add-in that includes a lot of special Interfaces, Types (Classes), Methods, and couple UI access utilities, that are custom to Inventor to make it easier for us to use for interacting with Inventor.
You can do way more with an iLogic rule than most would guess, because of being able to use all of the vb.net's already established capabilities.
For instance, since you mentioned Forms, I have created several iLogic rules that create their own Windows Form right in the same rule that is going to be using and reacting to the form. Here is a link to one of my earlier contribution posts, where I demonstrate this in an example. I know it's not as 'user friendly' to create them entirely by code, but it is an option.
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Wesley Crihfield
(Not an Autodesk Employee)
@Anonymous ,
@Anonymous wrote:But in these tests I found out that the iproperties.custom texts are also displayed on all other sheets. So "subject" of sheet 1 is also displayed on sheet 2 etc.
So this is not good, because sheet 2 has a different subject than sheet 1.
What exactly do you mean by "subject"?
You can edit the Title Block to show only what you want:
^In this case, you would edit what you want to show when you have Title Block 1 active. Then you do the same for all the other cases.
@Anonymous wrote:So I converted all sheet-dependent text / label to Prompted Entry's.
Now I've done kdit and then started testing again and then error messages pop up.
How can I fix this so that it works properly again?
You don't need to create entry's for something that Inventor will fetch from the model iProperties.
The best way to help you, would be if you could share the error message that pops up, as well as the drawing file you are using.
@Anonymous ,
I won't share the file you sent me, but leave here part of a solution, so others can use in the future.
The error you got was normal, since the Title Block couldn’t be placed because of the prompted entries on it.
I've got 2 workaround's.
- Input Box for every entry before placing the Title Block;
- Leave all prompted entries blank and fill them later;
1.
Dim oDoc As DrawingDocument = ThisApplication.ActiveDocument Dim oSheet As Sheet = oDoc.ActiveSheet Dim oTitleBlock As TitleBlock = oSheet.TitleBlock Try oTitleBlock.Delete Catch End Try 'Create as many as you need Dim oGetekend As String = InputBox("Getenked:", "Prompted Entries:") Dim oDatum As String = InputBox("Datum:", "Prompted Entries:") Dim oWijzigingletter As String = InputBox("Wijzigingletter:", "Prompted Entries:") Dim oAantal As String = InputBox("Aantal:", "Prompted Entries:") Try 'Change name between quotes to match your title block name ActiveSheet.SetTitleBlock("Test_stempel", oGetekend, oDatum, oWijzigingletter, oAantal) Catch 'Change name between single quotes to match your title block name MsgBox("No 'Test_stempel' found in this drawing!", , "Warning:") End Try
2.
Dim oDoc As DrawingDocument = ThisApplication.ActiveDocument Dim oSheet As Sheet = oDoc.ActiveSheet Dim oTitleBlock As TitleBlock = oSheet.TitleBlock Try oTitleBlock.Delete Catch End Try Try 'Change name between quotes to match your title block name 'Leave <""> as many as the number of entries you have ActiveSheet.SetTitleBlock("Test_stempel", "","","","") Catch 'Change name between single quotes to match your title block name MsgBox("No 'Test_stempel' found in this drawing!", , "Warning:") End Try
You can fill them later here:
I didn't had much time to work around on this.
Try it and give some feedback!