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!
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
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
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
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
Hello,
I am trying to follow what you guys have outlined on these threads and am having a bit of difficulty. I was able to get the rule working but cannot seem to get the rest of the way. I created the external iLogic rule and set the event trigger to "Before Save Document" like the basic iLogic thread said but when I open a part that was previously created, and click save, the iLogic rule does not run. It does show up in the iLogic browser as being available, but I thought that if it was created as an external rule it would run on any part when you click save even if you are trying to do it in a file that the rule was not created in.
Please help.
Mike
Mike,
Yes, you are correct about the external rule being able to run outside the part it was created in.
Is this box checked?
Yes that box is checked. So even though it is an external rule, it isn't a global setting? It is a per file setting?
Thank you for your help,
Mike
Mike,
In order for the external file to work, you have to set the trigger in EACH seperate part, idw or iam..... this is a local setting.
The "Run these rules when events occur" box is a global setting.
For the sheetmetal extents, I dont use ilogic. I prefer the Add-in method because I have legacy files that I need it to work with and I dont have a way to get the ilogic trigger set for those files.
Once this is installed, the addin will work for all sheetmetal parts and you dont have to set any triggers.... and it updates when the model changes (not saved).
Without using iLogic, is there a way to get this to report as a fraction of an inch?
Currently it shows it in decimal inches.
I know I'm johhny come (10 years) lately but I just worked the code above into my process.. so helpful, thankyou!
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