Hi everyone,
I would like to be able to the item number value that Inventor assigns to components in an assembly and feed these values down to the part level. Either to a parameter or i-property that I can then access at the part level and use as a text value to etch that value onto a part. Is this doable?
That helped! It worked. Now I'm trying to take use the FileName as well as the value stored under the ITEM custom iProperty and feed it to a parameter. I tried the following but I'm getting an error. I know it has to do with the syntax but how do I make the string combination read out as text in a parameter? I'm getting a conversion from string to type 'Double' error which I'm guessing has to do with the syntax I'm using.
Snip of Code:
FileName=ThisDoc.FileName(False) 'without extension
PartTag = FileName - iProperties.Value("Custom", "ITEM")
iLogicVb.UpdateWhenDone = True
This question may be a bit too obvious, but is that Parameter named "PartTag" a numerical parameter, or a text type user parameter? (It must be a text type user parameter for this to work.) When combining two String's together into one String in a line, you should use the '&' symbol between the first and next Strings. Using the '-' symbol without it being within quotes, invokes a mathematical operation. And since the iProperties call returns a generic 'Object' rather than a specific data Type, it is thinking that you are trying to do math between a String and an Object, which is not possible.
Try it like this:
FileName = ThisDoc.FileName(False)
'if you are expecting a String, then predefine the variable's Type as a String
Dim oItem As String = iProperties.Value("Custom", "ITEM")
'use '&' between Strings to join them
PartTag = FileName & oItemWesley Crihfield
(Not an Autodesk Employee)
Hi @amarinXG8V6. Actually, it looks like the last code that @dalton98 posted was attempting to incorporate the file name into the parameter, without using the iProperty, so it kind of sounds like that might have worked the way you wanted. This code below is basically just another very similar way of doing what his code was attempting to do, but I'm getting the file name a little differently, and avoiding use of the two Try...Catch blocks, in favor of a loop scenario. We have just assumed you wanted to go through 'Parts Only' view of the BOM because that is the tab being shown in your original image. If that needs to change too, that's not that difficult to change.
Dim oADoc As AssemblyDocument = ThisDoc.Document
oBOM = oADoc.ComponentDefinition.BOM
oBOM.PartsOnlyViewEnabled = True
oBOMView = oBOM.BOMViews.Item("Parts Only")
For Each oRow As BOMRow In oBOMView.BOMRows
Dim oPartDoc As PartDocument = oRow.ComponentDefinitions.Item(1).Document
'get file name, without path or file extension
oFileName = System.IO.Path.GetFileNameWithoutExtension(oPartDoc.FullFileName)
oItemNum = oRow.ItemNumber
oParamValue = oFileName & "-" & oItemNum
'now try to find the parameter within this part
oUParams = oPartDoc.ComponentDefinition.Parameters.UserParameters
Dim oPartTagParam As UserParameter = Nothing
For Each oParam As Inventor.Parameter In oParams
If oParam.Name = "PartTag" Then
oPartTagParam = oParam
oPartTagParam.Value = oParamValue
Exit For
End If
Next
If oPartTagParam Is Nothing Then
oPartTagParam = oUParams.AddByValue("PartTag", oParamValue, UnitsTypeEnum.kTextUnits)
End If
NextWesley Crihfield
(Not an Autodesk Employee)
That worked! One last question on this string. What if instead of gathering the filename I wanted to access the Project: Project i-property and combine that with the Part Only value from the assembly in a string. I assume I would chance the syntax for the portion of the code listed below. What would that syntax look like? Originally the intent was that the filename would be unique on a per project basis but based on my time studies, it would be better if we had a portion of the structural frame already modeled which would lend itself to more generic file names as opposed to project specific file names. That is why instead I think it would be best to use the Project: Project iProperty as a way to define which project the tube parts are associated with.
Thank you,
Alex
Hi @amarinXG8V6. If you want to replace file name with project iProperty value, we can do that fairly easily too. I would leave the line in place that gets the document object, because we can still use that to get the iProperty within that document.
Just replace this line:
oFileName = System.IO.Path.GetFileNameWithoutExtension(oPartDoc.FullFileName)with this line:
Dim oProject As String = oPartDoc.PropertySets.Item("Design Tracking Properties").Item("Project").ValueThen change this line:
oParamValue = oFileName & "-" & oItemNumto something like this:
oParamValue = oProject & "-" & oItemNum
Beware though...you may want to check to see if the Project iProperty has been filled in or not, just in case it is empty. I don't know if that would cause any problems if it were empty. To do so, you could just check if oProject = "". Then if it is empty, you could show yourself a message or use the iLogic Logger to write something to the log. Also beware of any 'virtual' components you may have in your BOM (if any), because they may not have a Document, which might cause an error.
Wesley Crihfield
(Not an Autodesk Employee)
I have updated the code to the following listed below, however when I run the rule I get the following error. Have I written something incorrectly?
Dim oADoc As AssemblyDocument = ThisDoc.Document oBOM = oADoc.ComponentDefinition.BOM oBOM.PartsOnlyViewEnabled = True oBOMView = oBOM.BOMViews.Item("Parts Only") For Each oRow As BOMRow In oBOMView.BOMRows Dim oPartDoc As PartDocument = oRow.ComponentDefinitions.Item(1).Document 'get file name, without path or file extension Dim oProject As String = oPartDoc.PropertySets.Item("Design Tracking Properties").Item("Project").Value oItemNum = oRow.ItemNumber oParamValue = oProject & "-" & oItemNum 'now try to find the parameter within this part oUParams = oPartDoc.ComponentDefinition.Parameters.UserParameters Dim oPartTagParam As UserParameter = Nothing For Each oParam As Inventor.Parameter In oParams If oParam.Name = "PartTag" Then oPartTagParam = oParam oPartTagParam.Value = oParamValue Exit For End If Next If oPartTagParam Is Nothing Then oPartTagParam = oUParams.AddByValue("PartTag", oParamValue, UnitsTypeEnum.kTextUnits) End If Next
I'm not sure what might be causing that error. Are there any virtual components in your assembly? Are you using any non-Master ModelStates settings? It seems like somewhere along the way, some variable is not getting a value set to it, then some other code is trying to use the variable without it having a value (or something like that). You will have to do some 'debug' type actions to help determine specifically where (what line of code) within the rule the error is being thrown. There are several ways to do that. (1)using the iLogic Logger to record a message between each action or line of code (2)putting something line MsgBox(1), MsgBox(2), MsgBox(3)... between each line of code, then watch the latest number message to show...the error is happening right after the last numbered message, (4) use Try...Catch blocks where something might possibly fail, with a message in the Catch part.
Wesley Crihfield
(Not an Autodesk Employee)
