iLogic Formual
Something like :
'Assuming that you have three custom Properties named "MegaThickness" , "MegaLength", and "MegaWidth" I believe this will do what you'd like
'
'Be sure to fill out the correct custom properties that you actually are using ;)
iProperties.Value("PartA:1", "Custom", "MegaThickness") = Measure.ExtentsHeight
iProperties.Value("PartA:1", "Custom", "MegaLength") = Round(Measure.ExtentsLength,2)
iProperties.Value("PartA:1", "Custom", "MegaWidth") = Round(Measure.ExtentsWidth,2)
iProperties.Value("PartA:1", "Project", "Stock Number") = _
iProperties.Value("PartA:1", "Custom", "MegaLength") & " X " & iProperties.Value("PartA:1", "Custom", "MegaWidth")
Does that help you?
If my solution worked or helped you out, please don't forget to hit the kudos button 🙂
iLogicCode Injector: goo.gl/uTT1IB
The code that I posted should be ran from the assembly, and works. Did you actually try using it? Is the problem now that you would like to update all of the parts (and in turn : iProperties) that are in the assembly ?
The code you last posted could work with some tweaking, but I don't believe that it will work in that current state.
If my solution worked or helped you out, please don't forget to hit the kudos button 🙂
iLogicCode Injector: goo.gl/uTT1IB
Hi andrew.warren,
Here is some information on creating the custom prop if it does not exist:
http://inventortrenches.blogspot.com/2011/05/use-ilogic-to-add-and-use-custom.html
Also just a heads up, I took a couple of minutes to look at your overall goal, an noticed that Measure.ExtentsHeight runs on the top level assembly (and therefore gathers it's height) even when iterating through the assembly components via the For Each. Unfortunately I didn't find a solution, but will post back I think of something.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'Define the open document
Dim openDoc As Document
openDoc = ThisDoc.Document
Dim docFile As Document
For Each docFile In openDoc.AllReferencedDocuments
'format file name
Dim FNamePos As Long
FNamePos = InStrRev(docFile.FullFileName, "\", -1)
Dim docFName As String
docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)
customPropertySet = docFile.PropertySets.Item _
("Inventor User Defined Properties")
'check for custom iprops and add them if not found
Try
prop1 = customPropertySet.Item(“Thickness")
prop2 = customPropertySet.Item(“Width")
prop3 = customPropertySet.Item(“Length")
Catch
' assume error means not found
customPropertySet.Add("", “Thickness")
customPropertySet.Add("", “Width")
customPropertySet.Add("", “Length")
End Try
'get value from model
prop1.value = Measure.ExtentsHeight
prop2.value = Measure.ExtentsWidth
prop3.value = Measure.ExtentsLength
Next
Hi andrew.warren,
What you have works, but I noticed an issue that might trip you up.
If the iprops are checked and added as a group, it could cause an error if one of them exists but the others don't. So here's a version that checks/adds them one at a time. I've also added the measure extents to the check/add step, so that it just fills in the value as it the iProperty is checked/created.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Dim docFile As Document
docFile = ThisDoc.Document
customPropertySet = docFile.PropertySets.Item _
("Inventor User Defined Properties")
'check for custom iprop and add if not found
Try
customPropertySet.Item(“Thickness").Value = Measure.ExtentsHeight
Catch
' assume error means not found and add
customPropertySet.Add(Measure.ExtentsHeight, “Thickness")
End Try
'check for custom iprop and add if not found
Try
customPropertySet.Item(“Width").Value = Measure.ExtentsWidth
Catch
' assume error means not found and add
customPropertySet.Add(Measure.ExtentsWidth, “Width")
End Try
'check for custom iprop and add if not found
Try
customPropertySet.Item(“Length").Value = Measure.ExtentsLength
Catch
' assume error means not found and add
customPropertySet.Add(Measure.ExtentsLength, “Length")
End Try
I'm going to add this just in case someone might find it helpful, or in case this can be used to find a solution to getting the size for each component in the assembly. This rule does pretty much the same thing the other does, but as written it writes the extents info all to one custom iProperty named Size (example: Size: 0.3 in. x 0.3 in. x 0.3 in.) It also formats the length of the size string. (example: 0.25 becomes 0.3 in. )
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'check for custom iprops and add them if not found
Dim propertyName1 As String = "Size"
customPropertySet = ThisDoc.Document.PropertySets.Item _
("Inventor User Defined Properties")
Try
prop = customPropertySet.Item(propertyName1)
Catch
' Assume error means not found
customPropertySet.Add("", propertyName1)
End Try
' Get the active document. This assumes it is a part document.
Dim oPartDoc As PartDocument
oPartDoc = ThisApplication.ActiveDocument
Dim oBox As Box
oBox = oPartDoc.ComponentDefinition.SurfaceBodies.Item(1).RangeBox
'set IncludeLeadingDigit option
'optional
'use TriState.True to return a number such as 0.123
'use TriState.False to return a number such as .123
'use TriState.UseDefault to use the computer's regional settings
LeadZero = TriState.True
'set NumDigitsAfterDecimal option
'optional
DecNum = 1
'set UseParensForNegativeNumbers
'optional
'use TriState.True to return a negative number as: (49.123)
'use TriState.False to return a negative number as: -49.123
'use TriState.UseDefault to use the computer's regional settings
NegFormat = TriState.False
'set GroupDigits to include group delimiter specified (as specified in the locale settings)
'optional
'use TriState.True to return a number as: 1,234 (where comma is the locale setting)
'use TriState.True to return a number as: 1234
'use TriState.UseDefault to use the computer's regional settings
GroupDigits = TriState.False
Length1 = (oBox.MaxPoint.X - oBox.MinPoint.X) * 0.394 '& " in."
Width1 =(oBox.MaxPoint.Y - oBox.MinPoint.Y) * 0.394 '& " in."
Thickness1 = (oBox.MaxPoint.Z - oBox.MinPoint.Z) * 0.394 '& " in."
Length = FormatNumber(Width1, DecNum, LeadZero, NegFormat, GroupDigits)
Width = FormatNumber(Length1, DecNum, LeadZero, NegFormat, GroupDigits)
Thickness = FormatNumber(Thickness1, DecNum, LeadZero, NegFormat, GroupDigits)
'MessageBox.Show("Extents = " & Thickness & " in. x " & Length & " in. x " & Width & " in. " , "Title")
iProperties.Value("Custom", "Size") = Thickness & " in. x " & Length & " in. x " & Width & " in. "
I have implemented this rule but i'm stumbling upon an exception of use for this rule.
Suppose you have created your part with the use of "Make Components", nothing wrong with that but, ... (And this is where i have found the "exception", if your part is not designed perpendicular to at least 2 of the axis X,Y or Z, you get wrong results.
An example:
Suppose picture below (you'll get the idea instantaneously 😉 )
Now according to common sense my bounding box should be 10 x 50 x Height, but when i apply the rule to this part, my bounding box becomes :
Any ideas on how to overcome this?
Change UCS on demand of the Bounding Box?