Okay, I'm sure iLogic can do this, but what snippet is used when I need to make a parameter in my open doc. equal the parameter in another doc... that is not included in the active assembly?
Can iLogic look at a part that is not included in the active assembly?
I found the "path", "Filename", "Pathandfilename"...
just not sure how to make them work.
I just need to make it look into another folder... also, does the part I'm looking at have to be in the "active" project
Hi @chris,
First, remember that there is an Inventor Customization forum that is probably a better place to post ilogic and programming questions :
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/bd-p/120
Second, understand that there are straight ilogic functions and then there are API (application programming interface) calls that we often use with ilogic to go beyond the simple set of iLogic functions. I mention this because most of the iLogic functions are intended to work with the current active document, and/or to reach through the current active document into it's referenced files.
So with all of that in mind for the future, to get back to your question, the answer is yes, if we know the path and filename of the file we want to access, then we can open it into the session of Inventor and write to it's iprops, and then save and close it.
Here is a quick example that combines ilogic functions and API calls to open a file invisibly from a hard coded file path and name, then shows the existing part number, gets a new part number, and saves and closed the file. More typically we'd determine path and file name more dynamically, but sometimes it might be static like this simple example.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
sFolder = "C:\TEMP\"
sName = "A100-02.ipt"
sFile = sFolder & sName
'open the file, false opens the file without generating the graphics
oDoc = ThisApplication.Documents.Open(sFile, False)
'get part number iProp
oPN = iProperties.Value(oDoc, "Project", "Part Number")
'show existing part number
MessageBox.Show(oPN, "iLogic")
'get user input
oPN = InputBox("Enter new Part Number", "iogic", oPN)
'write user input to part number iProp
iProperties.Value(oDoc, "Project", "Part Number") = oPN
'close doc, True saves the doc on close
oDoc.Close(True)
The existing documentation is great for this.... :
And to answer your other question: NO, iLogic cannot access files that are not a direct child of the open document.
Sadly, I've tested a couple cases and found:
- You cannot even use the file name to access the top level file to assign an iProperty as it causes an error. (iProperties.Value(System.IO.Path.GetFileName(ThisDoc.Document), "Project", "Part Number") is an example that fails)
- You cannot use the file name to access the drawing of the current part, even if it is open. (Using a similiar call to above, but changing the file name)
If you were to want to do this, you would have to use the API directly such as:
oSourceDoc = ThisApplication.Documents.Open("C:\SourceFile.ipt",False)
oSourceParams = oSourceDoc.ComponentDefinition.Parameters
Try
oLen = oSourceParams("Length").Value
Parameter("Length") = oLen
Catch
MsgBox("Error Assigning Parameter.")
End Try
oSourceDoc.Close
@chris wrote:
My current project is an automated assembly, so all parts in the assembly reference back to a base part, but if I create a new parameter at the base part, I then have to go into every other part and "update" the linked component to see the new parameter...
Also, see this link, it pushes all of the custom parameters in the assembly to all of the referenced parts:
From your earlier description I'm unsure if your "base part" is referenced or not, but if so, something like the example at that link is probably the way to go.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
