Suppress occurrence of pattern with iLogic

[fakeru]

Hello!

Is it possible to suppress an occurrence of a pattern in part enviroment using iLogic? I saw something for aseembly enviroment, but I can't make it work for part. My iLogic knowledge is quite basic.

If you have a rule for this, please help me!

Regards

[CCarreiras]

Hi!!

I think is not possible because the software can't guess which occurrence to suppress.

Instead, you may create several Patterns, each one with the propper configuration, and use ilogic to supress the Patterns you don't need for each specific case.

Regards

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[Telson.Hadden]

Yes, it is possible.  difficult, but possible - and you have to be careful not to try to change the suppression on the first item, because it will error out without telling you why.

 Dim oPattern As RectangularPatternFeature 
 oPattern = ThisDoc.Document.ComponentDefinition.Features.RectangularPatternFeatures.Item("<pattern name>")
 
 Dim oElement As FeaturePatternElement
 
 	For Each oElement In oPattern.PatternElements
		if oElement.index = 1 then
			'do nothing - you're not allowed
		else
			oElement.suppressed = True 'or false
		end if
	Next 
ThisDoc.Document.update

I know this is an old post, but they are everywhere, with no solution to be found.

[serpennica]

Inventor 2017

I'm working with a "sketch driven pattern" in a part.

Was looking at the script and only got the whole

 pattern to suppress. Was not able to get individual occurrences suppressed.

how do we get the 5, 6,7 occurrence to suppress.

have not seen much on this, mostly with assemblies,

any help, thanks Sergio 

[bradeneuropeArthur]

Please read your last topic.

And

https://www.cadlinecommunity.co.uk/hc/en-us/articles/210054325-Inventor-2017-quick-tip-Set-rules-to-...

Regards,

Autodesk Software: Inventor Professional 2018 | Vault Professional 2018 | Autocad Mechanical 2018
Programming Skills: Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
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! For administrative reasons, please mark a "Solution as solved" when the issue is solved !

[serpennica]

the option of pattern properties is not what i was looking for.

that option only gives me an if statement to suppress the whole pattern.

I was looking to suppress the occurrences one at a time.

thanks for the help.

[DRoam]

---

@serpennica wrote:

Was looking at the script and only got the whole

 pattern to suppress. Was not able to get individual occurrences suppressed.

how do we get the 5, 6,7 occurrence to suppress.

have not seen much on this, mostly with assemblies,

---

This isn't a question of part vs. assembly, it's simply a question of programming. There are many ways to only suppress those occurrences. Probably a Select Case is one of the simpler methods:

Dim oPattern As RectangularPatternFeature 
oPattern = ThisDoc.Document.ComponentDefinition.Features.RectangularPatternFeatures.Item("<pattern name>")
 
For Each oElement As FeaturePatternElement In oPattern.PatternElements
	Select Case oElement.index
		Case 5,6,7
			oElement.suppressed = True 'or false
	End Select
Next

ThisDoc.Document.update

[DRoam]

Actually, to suppress specific elements, you don't even need to iterate through the elements. You can suppress them directly like this:

Dim oPattern As RectangularPatternFeature
oPattern = ThisDoc.Document.ComponentDefinition.Features.RectangularPatternFeatures.Item("<pattern name>")
 
Dim oElements As FeaturePatternElements = oPattern.PatternElements

oElements(5).Suppressed = True
oElements(6).Suppressed = True
oElements(7).Suppressed = True

ThisDoc.Document.update

[serpennica]

Perfect. That was it.

changed the rectangular pattern to sketch driven pattern and used a function to drive the true/false. now I can get a dialog box "forms" to select the element i want to remove.

thank you.

[serpennica]

Perfect. That was it.

changed the rectangular pattern to sketch driven pattern and used a function to drive the true/false. now I can get a dialog box "forms" to select the element i want to remove.

thank you.