topic Re: ilogic sketch text in Inventor Programming Forum

ilogic sketch text

Cosmin_V — Mon, 10 May 2021 09:22:33 GMT

I have this code in one part, and it works ok.
But If I try to control the text from an assembly,
"I did a "Text Parameter" in assembly "Engraving"and that parameter is = whit a "Text Parameter" in part "EngravingL" from part and "EngravingL" it shoud be the text in the sketch."
I get this error.

Dim oPartDoc As PartDocument
Dim oTextbox As TextBox
    oPartDoc = ThisApplication.ActiveDocument
Dim oCd As ComponentDefinition
Dim oSketch As PlanarSketch

For Each oCd In oPartDoc.ComponentDefinitions
    For Each oSketch In oCd.Sketches
        For Each oTextbox In oSketch.TextBoxes
			oTextbox.Text = EngravingL
        Next
    Next
    
Next

Can anyone help me?

Re: ilogic sketch text

bradeneuropeArthur — Tue, 11 May 2021 08:11:59 GMT

Are you sure that the code runs only in the part and not in the assembly?

Re: ilogic sketch text

Cosmin_V — Tue, 11 May 2021 12:33:57 GMT

The code is set in part.

As it is now, it doesn't work in the assembly. Maybe with some adjustments ... I would like it more if it worked from assembly

Re: ilogic sketch text

Curtis_W — Tue, 11 May 2021 16:17:26 GMT

Hi @Cosmin_V

This worked for me to set the textbox value of each assembly sketch.

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

Dim oDoc As Document Dim oTextbox As TextBox oDoc = ThisApplication.ActiveDocument Dim oCd As ComponentDefinition Dim oSketch As PlanarSketch For Each oCd In oDoc.ComponentDefinitions For Each oSketch In oCd.Sketches For Each oTextbox In oSketch.TextBoxes oTextbox.Text = "Test" Next Next Next

Re: ilogic sketch text

WCrihfield — Tue, 11 May 2021 16:42:29 GMT

Do you want to work with all local iLogic rules, or do you prefer external iLogic rules for this solution?

What action do you want to trigger the sketch text to change? Do you just want to run a local rule within the main assembly to make it all happen? Or maybe you want it so that when you change the value of the text parameter in the assembly, it causes a local rule within the assembly to run that will push that value to the part, then run a rule in the part to change the text in the sketch? It will be easier to set-up the parameter change triggering if you are using local rules in both cases, but it can also be done using external rules if needed (just requires more work/set-up).

If using local rules, and you want the change to happen when you change the parameter value within the main assembly, here is some example local iLogic rule codes you can try:

Within the main assembly document, create a new rule and copy/paste this following code into it. You will need to change the path & file name to the target Part file, or get the Part file in another way, if needed. (You can delete the comments, once you get it working OK.)

'try to specify/find/get the target part document 'it should already be 'initiated' because it's within the assembly, so we don't need to specifically open it Dim oPDoc As PartDocument Try '<<<< CHANGE THIS PATH & FILE NAME >>>> 'or get the part document another way, if needed oPDoc = ThisApplication.Documents.ItemByName("C:\Temp\MyPart.ipt") Catch MsgBox("Couldn't find the Part document named 'MyPart.ipt'. Exiting.") Exit Sub End Try Dim oPrtParam As Inventor.Parameter Try oPrtParam = oPDoc.ComponentDefinition.Parameters.Item("EngravingL") Catch MsgBox("Couldn't find the parameter named 'EngravingL' within the Part. Exiting.") Exit Sub End Try 'set the value of the part's parameter to the value of the assemblies parameter 'when using a 'blue' local parameter name, it will trigger this rule to run when its value changes oPrtParam.Value = Engraving 'local' parameter (should turn blue) within the Assembly

Then within the Part document, change its local rule code to this:

Dim oPDoc As PartDocument = ThisDoc.Document 'points to the 'local' document Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition For Each oSketch As PlanarSketch In oPDef.Sketches For Each oTextBox As Inventor.TextBox In oSketch.TextBoxes oTextBox.Text = EngravingL 'local parameter (should turn blue) Next Next

You may have to update the part and/or assembly after wards to see the changes, or simply include an extra line of code in them to RebuildAll or Update.

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Re: ilogic sketch text

Curtis_W — Tue, 11 May 2021 17:34:38 GMT

Hi @Cosmin_V

After reading WCrihfield's reply it occurred to me that you might be wanting to set the text in the sketches of all parts from the assembly.

Here are a couple more examples.

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

This sets the same text to all parts

Dim oAsmDoc As AssemblyDocument oAsmDoc = ThisApplication.ActiveDocument oText = InputBox("Enter Text:", "iLogic", "Test") Dim oDoc As Document For Each oDoc In oAsmDoc.AllReferencedDocuments If oDoc.DocumentType = kPartDocumentObject Then Dim oCd As ComponentDefinition Dim oSketch As PlanarSketch For Each oCd In oDoc.ComponentDefinitions For Each oSketch In oCd.Sketches For Each oTextbox In oSketch.TextBoxes oTextbox.Text = oText Next Next Next End If Next InventorVb.DocumentUpdate()

This sets each part to use a different entered text value

Dim oAsmDoc As AssemblyDocument oAsmDoc = ThisApplication.ActiveDocument Dim oDoc As Document For Each oDoc In oAsmDoc.AllReferencedDocuments If oDoc.DocumentType = kPartDocumentObject Then Dim oCd As ComponentDefinition Dim oSketch As PlanarSketch For Each oCd In oDoc.ComponentDefinitions For Each oSketch In oCd.Sketches For Each oTextbox In oSketch.TextBoxes oText = InputBox _ ("Enter Text for " & oDoc.DisplayName, "iLogic", oTextbox.Text) oTextbox.Text = oText Next Next Next End If Next InventorVb.DocumentUpdate()

And here is an example that looks for a parameter in all the occurences named EngravingL and sets that if it is used (this assumes that parameter is being called into the text box)

Dim oAsmDoc As AssemblyDocument oAsmDoc = ThisApplication.ActiveDocument oText = InputBox("Enter EngravingL text:", "iLogic", "Test") Dim oOcc As ComponentOccurrence For Each oOcc In oAsmDoc.ComponentDefinition.Occurrences Try Parameter(oOcc.Name, "EngravingL") = oText Catch 'error when parameter not found End Try Next InventorVb.DocumentUpdate()

Re: ilogic sketch text

Cosmin_V — Wed, 12 May 2021 13:24:43 GMT

Hi everyone

No one works! 😞

It is a 4-piece ensemble. 3 have the same engraved code, and one another code.

I have set the code (from the first post) in all parts.

And I create a "Text parameter" in each part. (EngarvingL) which should be engraved on each part.

And in assembly I create 2 "Text parameter" "Engarving_Finger_Text" and "Engarving_Plate_Text"

And a rule ...

Parameter(o00292307.Name, "EngravingL")  = Engraving_Finger_Text
Parameter(o00292308.Name, "EngravingL") = Engraving_Finger_Text
Parameter(o00292309.Name, "EngravingL") = Engraving_Finger_Text
Parameter(o00292310.Name, "EngravingL")  = Engraving_Plate_Text

And I put in form the parameters

Engraving_Finger_Text
Engraving_Plate_Text

Re: ilogic sketch text

Cosmin_V — Wed, 12 May 2021 13:39:08 GMT

this is the error

Re: ilogic sketch text

Curtis_W — Wed, 12 May 2021 15:04:20 GMT

Hi @Cosmin_V

If I put this rule in the assembly, it will update the parameter called EngravingL in the part file... when that parameter is used in the part sketch it will update to show both assembly parameter values, when those value are updated from the assembly form.

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

Dim oAsmDoc As AssemblyDocument oAsmDoc = ThisApplication.ActiveDocument oTrigger = Engarving_Finger_Text oTrigger = Engraving_Plate_Text Dim oOcc As ComponentOccurrence For Each oOcc In oAsmDoc.ComponentDefinition.Occurrences Try 'set the parameter value in the part Parameter(oOcc.Name, "EngravingL") = _ Parameter("Engarving_Finger_Text") & " " & Parameter("Engraving_Plate_Text") Catch 'error when parameter not found End Try Next InventorVb.DocumentUpdate()

Re: ilogic sketch text

Cosmin_V — Mon, 17 May 2021 08:00:53 GMT

Thank you very much!

But whatever I do, I get this error! 😞

Error in rule: Rule0, in document: 00292309.ipt

Unable to cast COM object of type 'System.__ComObject' to interface type 'Inventor.PartDocument'. This operation failed because the QueryInterface call on the COM component for the interface with IID '{29F0D463-C114-11D2-B77F-0060B0F159EF}' failed due to the following error: No such interface supported (Exception from HRESULT: 0x80004002 (E_NOINTERFACE)).

Re: ilogic sketch text

Cosmin_V — Mon, 17 May 2021 11:07:30 GMT

I fixed it...

I change....

oPartDoc = ThisApplication.ActiveDocument

Whit ....

oPartDoc = ThisDoc.Document

Re: ilogic sketch text

WCrihfield — Mon, 17 May 2021 17:26:10 GMT

Glad to hear you got it working OK. Issues involving multiple documents and multiple iLogic rules can sometimes be challenging for others to diagnose remotely. Here is a link to one of my contribution posts that I think you'll find interesting/helpful, that sort of relates to the problem you were having with the document reference. It attempts to help explain most of the different document references, and when/where they are best used. Good luck in your future iLogic endeavors.