Not enough memory resources are available to complete this operation

[Mikeclarke1500]

we have a template we created for supressing instances of a pattern outside of a boundary sketch. originally from mod the machine blog but the ilogic code was written by an autodesk employee.

it's worked fine for a long while but recently got an error message - "Not enough memory resources are available to complete this operation". I have attached screenshot of the message and more info.

for info the part is a flat rectangular plate with a pattern of 5000 holes. 

is there a way to increase the memory available for inventor to use? any other solutions?

PC is very good, 12th gen i9 and 64gb RAM

[kacper.suchomski]

Hi

Check this: File -> Options -> General -> Undo file size (MB) -> 8191

[Mikeclarke1500]

hi Kacper, thanks for the response. unfortunately I changed the undo size and still get the error. 

is there any other solutions? I just tried to make it higher but it seems 8191 is the max.

[Anonymous]

Clear out your temp files?

That need seems to be a weekly deal these days.

[johnsonshiue]

Hi! This could be related to the graphics RAM. How much graphics RAM does the machine have? Please share the file and the iLogic rule. I would like to understand it better. It could also be a bug.

Many thanks!

[Mikeclarke1500]

hi Johnson, I have uploaded the file for you and it should include the ilogic rule.

thanks

[Mikeclarke1500]

FYI I have cleared out temp files and still have the issue

[MjDeck · Accepted solution]

Hi @Mikeclarke1500 - thanks for reporting this. It turns out that the error message is misleading: the problem is not really related to memory. It's more like an "operation not supported" issue. It occurs when the rule tries to project a Spline Handle in your Boundary sketch. That is easy to work around, but the rule has other problems with a large number of occurrences in the pattern.

In Inventor 2025, you can edit a rectangular pattern and select a boundary sketch to trim it to. No iLogic rule is required.

I attached a different rule. This will work on your part in Inventor 2024. To use it, copy the attached PatternWithinBoundary.txt to one (and only one) of these locations:

• the same folder as the part
• your project workspace folder
• your External Rules Directory (as set in Tools > Options > dropdown at bottom > iLogic Configuration)

Then edit your part. Rename the Suppress_Extra_Holes rule and create a new Suppress_Extra_Holes rule with this text:

AddVbFile "PatternWithinBoundary"
Sub Main
	Dim pwb As New PatternWithinBoundary(ThisDoc.Document, ThisServer)
	
	pwb.ClipPattern("Hole2", "HolesArray", "Boundary", 0.0)
	
	iLogicVb.DocumentUpdate
End Sub

That should work.
Note that some edges of pattern elements might cross the boundary. It's only checking the center point of each pattern element. If you want to keep them away from the boundary, you can set the value of the offset argument (which is 0.0 in the sample above).