iLogic, make extrusion on Flat Pattern

[Rob67ert]

I like to make an extrusion of a sketch that is placed on the flat pattern.

What i now have is:

SyntaxEditor Code Snippet

Dim oDoc As PartDocument = ThisDoc.Document
Dim oDef As SheetMetalComponentDefinition = oDoc.ComponentDefinition
Dim oSK As Sketch = oDef.FlatPattern.Sketches(1)
Dim oProfile As Profile = oSK.Profiles.AddForSolid
Dim oExtrudeDef As ExtrudeDefinition = oDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kJoinOperation)
Call oExtrudeDef.SetDistanceExtent(0.25, kPositiveExtentDirection)
oExtrude = oDef.Features.ExtrudeFeatures.Add(oExtrudeDef)

But this makes the extrusion on the Sheetmetal and not on the Flat pattern...

Does anyone have an idea how i can make this work correct?

[MechMachineMan]

Your oDef is the folder part model. You tell it to put the features on the folded part model according to your rule.

You need to use oDef.Flatpattern as that is also a sheetmetalcomponentdefinition, but is the one responsible for the flat pattern.

If that still doesn't work, you may actually have to activate the part for edit in flat pattern mode.

Good luck.

[bshbsh · Accepted solution]

You have to create the ExtrusionDefinition and the Extrusion feature on the Flatpattern, not on oDef (which is the folded sheetmetal definition.)

so basically replace all oDef.Features with oDef.FlatPattern.Features:

Dim oDoc As PartDocument = ThisDoc.Document
Dim oDef As SheetMetalComponentDefinition = oDoc.ComponentDefinition
Dim oSK As Sketch = oDef.FlatPattern.Sketches(1)
Dim oProfile As Profile = oSK.Profiles.AddForSolid
Dim oExtrudeDef As ExtrudeDefinition = oDef.FlatPattern.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kJoinOperation)
Call oExtrudeDef.SetDistanceExtent(0.25, kPositiveExtentDirection)
oExtrude = oDef.FlatPattern.Features.ExtrudeFeatures.Add(oExtrudeDef)

[Rob67ert]

I know that is had to be something like that.

Thanks.