Autodesk Inventor

[#1]

I am using IV ultimate 2013

Hi just found about this add-in:http://modthemachine.typepad.com/my_weblog/2012/05/sheet-metal-extents-add-in-update.html

But its not working for me:

I ran the installer

created a sheet metal part and hit rebuild all, it did not create any proeprties, also tried to manually create the properteis then hit rebuild, no go.

I also did a search on my hardrive for the ApplicationPlugins, and placed the sheet metal folder in all of them(there were 3)

tried again noto.

The add-in also does not appear in the add-in manager.

Any Ideas

Or is there differnt wat to get the flat pattern dimensions in 2013

TIA!

[#2]

Hi omartin,

If your goal is to show the flat pattern extents on the drawing then indeed this is built into Inventor now. You can do so by using the Text tool and pulling the Sheet Metal Properties as shown here.

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

[#3]

Hey Curtis thanks for they reply.

But I plan on showing it in the BOM, Ideally it would be in the fxParameters (which I think this add-in supports)

But I have some custom variables in my BOM that I use, and I am hoping I can point to those custom properties.

I will keep on trying to figure it out.

Regards

[#4]

Hi omartin,

If it helps, you can create a simple iLogic rule to place the extents information into custom iProperties that can be used in the BOM & Parts List. Attached is example with the rule placed in the part, but I'd recommend creating the rule as an external rule, so you can have it run on all sheet metal parts when they are saved, etc.

http://inventortrenches.blogspot.com/2012/01/creating-basic-ilogic-rule-with-event.html

Dim oDoc As Document
oDoc = ThisApplication.ActiveDocument

'make sure the part is a sheet metal part
If oDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then 
MessageBox.Show("This is not a sheet metal part.", "iLogic")
Return 'exit rule
Else 

Dim oSMDef As SheetMetalComponentDefinition
oSMDef = oDoc.ComponentDefinition

Dim sExtLength As String = "extents_length"
Dim sExtWidth As String = "extents_width"
Dim sExtArea As String = "extents_area"
Dim iRoundValue as Integer = 2
 
'check for flat pattern
If oSMDef.FlatPattern Is Nothing Then 
'create a flat pattern if it doesn't exist
oSMDef.Unfold
oSMDef.FlatPattern.ExitEdit
Else

'define custom property set
customPropertySet = ThisDoc.Document.PropertySets.Item _
("Inventor User Defined Properties")

'look for custom iproperty and try to set it
Try
          iProperties.Value("Custom", sExtLength) = Round(SheetMetal.FlatExtentsLength, iRoundValue)
Catch
' assume error means not found and create it
            customPropertySet.Add(Round(SheetMetal.FlatExtentsLength,iRoundValue), sExtLength)
End Try

'look for custom iproperty and try to set it
Try
          iProperties.Value("Custom", sExtWidth) = Round(SheetMetal.FlatExtentsWidth,iRoundValue)
Catch
' assume error means not found and create it
            customPropertySet.Add(Round(SheetMetal.FlatExtentsWidth,iRoundValue), sExtWidth)
End Try

'look for custom iproperty and try to set it
Try
          iProperties.Value("Custom", sExtArea) = Round(SheetMetal.FlatExtentsArea,iRoundValue)
Catch
' assume error means not found and create it
            customPropertySet.Add(Round(SheetMetal.FlatExtentsWidth,iRoundValue), sExtArea)
End Try

End if
End If

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

[#5]

Curtis,

How can I get this information (extents_length and Extents_width) to be written to the model user parameters instead of the custom iProperty parameters?

Thanks

[#6]

Curtis wrote the iLogic code to get put this information in the User Parameters. Here is the thread that discussed doing this.  The code is attached below.