ilogic turn off/on drawing view depending of surpressing status in assembly file

[Anonymous]

Hello Autodesk Community,

I have to create a drawing wich shows me every part of an assembly, depending on if its active or surpressed.

Ive allready tryed the View.is.active funktion and set it to an "if" to component.is.active dialog in the .idw file.

This dosnt work- error "can t use component is active in an .idw"

Tryed to add a View of the assembly in the same Drawing (may id would get any reference)-also not working

For ease: I create a .idw wich contains every part of my .iam switch the views on/off depending of their surpressing status in the .iam file.

May i can trigger it with an parameter dialog to the .idw file?..."if para=1 view is active"..im not sure

Background: For our Laser it would be usefull to get every part on a single .dxf.

After getting the parts in one single Drawing the creation of the .dxf file by ilogic would be no problem.

After among 6 month of reading the posts in this Forum (and others thx curtis) im allready at the end of the Road.

Wich means there is such an huge resource of ideas and code in here that i dont have to ask anything!..........thanks to you all!!!Great work!!!

May (sure) you can help me with my issue.

excuse my texting - its not my mothertoungue

Simon

[Owner2229]

Hi, are all the parts in one drawing view (placed as assembly)? Or each part has it's own view?

If it is the first case, then you don't even need iLogic, you can do it like this:

In open drawing double click the view you want to "link" to the assembly.

Change the "View representation" to "Default".

There's litle check box with "chain" symbol next to it, change it to be "checked".

Change the "Level of Detail" to match your assembly's one.

Now you can try to play with your assembly and the drawing will update.

[Anonymous]

Thanks for Reply,

Its the second case, every part has its own View. Quite a batch of the parts i need to cut by the laser.

Thanks for your solution but it will not work for my case.

[Anonymous]

Can you post your code thus far and/or a sample assembly to test with?

[Anonymous]

I would need something like this:

SyntaxEditor Code Snippet

If Component.IsActive("RK_EK.iam","SL:1") = True Then
ActiveSheet.View("ANSICHT9").View.Suppressed = False
Else
ActiveSheet.View("ANSICHT9").View.Suppressed = True
End If

So i place every part of my .iam in the drawing and surrpress/unsurrpress the view, depending of the status in the .iam....

But this dosent work, i need a connection to the .iam file?......but how? 

thanks for reply 

[Anonymous]

See if this works:

'Define the open Document
Dim openDoc As Document
openDoc = ThisDoc.Document


'Look at the model file referenced in the open document
Dim docFile As assemblyDocument
docFile = ThisDoc.ModelDocument
Dim oAsmCompDef As ComponentDefinition
oAsmCompDef = docFile.ComponentDefinition

If ThisDoc.ModelDocument IsNot Nothing Then

Dim oCompOcc As Inventor.ComponentOccurrence
For Each oCompOcc in oAsmCompDef.Occurrences

On Error Resume Next

'if component is "RK_EK.iam","SL:1" check if enabled, if not suppress corresponding view'--- copy for each part in assembly

'--- Copy for each part/view 
If oCompOcc.Name = "RK_EK.iam","SL:1" Then
	If oCompOcc.Enabled = True Then 
		ActiveSheet.View("VIEW3").View.Suppressed = True
	Else
		ActiveSheet.View("*VIEW NAME*").View.Suppressed = False
	End If
End If
'--- Copy for each part/view 

Next
 


End If

Subsitute the part and view names were needed.

This is mostly from memory and untested, so see how you get on and come back to me with any errors.

[Anonymous]

Thanks Neil,

this could work!

but sadly I got an error in the

If oCompOcc.Name = "RK_EK.iam","SL:1" Then

Line,  but i thinks this is an copy/paste problem, or forgot an END comand?

Thanks for help

[Anonymous]

Hi,

I think the error is like you said a copy.paste issue.

the oCompOcc.Name need to reflect exactly what is in your feature tree.

so if the part in your tree says Top Plate:1 then the code needs to read :

If oCompOcc.Name = "Top PLate:1" then





End if

see if that fixes it.

[Anonymous]

No...I think the Problem is by copy the code snippet.

Get an error that means i have to ad an end funktion after if.

[Anonymous · Accepted solution]

This is a straight copy from a test assembly/drawing I made up and it worked sucessfully on:

if you've put this into a new drawing file to test it make sure and save it first.

'Define the open Document
Dim openDoc As Document
openDoc = ThisDoc.Document


'Look at the model file referenced in the open document
Dim docFile As assemblyDocument
docFile = ThisDoc.ModelDocument
Dim oAsmCompDef As ComponentDefinition
oAsmCompDef = docFile.ComponentDefinition

If ThisDoc.ModelDocument IsNot Nothing Then

Dim oCompOcc As Inventor.ComponentOccurrence
For Each oCompOcc in oAsmCompDef.Occurrences

On Error Resume Next

'if component is "***" check if enabled, if not suppress corresponding view'--- copy for each part in assembly

'--- Copy for each part/view 
If oCompOcc.Name = "SCW15498-03004 Backplate:1" Then
	If oCompOcc.Enabled = True Then 
		ActiveSheet.View("VIEW3").View.Suppressed = True
	Else
		ActiveSheet.View("VIEW3").View.Suppressed = False
	End If


	End If
'--- Copy for each part/view 

Next
 
End If

see how my component name is not the file name put the name that shows up in the assembly tree, including the :1 suffix.

EDIT:

Find attached my test assembly and drawing with  internal rule .

You'll see that View3 is already suppressed as the rule says.

[Anonymous]

THX....works fine