Disable plot ability for a part?

[llorden4]

I've got an assembly template I'm pre-building for a number of drafting teams and one of the features I'm trying to include is a reference part that provides a visual inspection for fit of a complex pattern assembly that repeats.  I'm able to configure the part to stay out of the BOM's, have zero mass properities, but I also want to prevent the part from plotting on any drawing files generated.  Think of of this part as a go/no-go jig you'd hand to you production crews.  Is there any method to flag a part to be non-printable yet remain visible to the drafter; comparable to placing an object on the Defpoints layer in AutoCAD?

[HideoYamada]

Hello,

Have you tried using Design View Representation?

[llorden4]

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@HideoYamada wrote:

Hello,

Have you tried using Design View Representation?

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I'm familiar with the feature, basically a named view that turns the visibility of objects on and off.  Since I'm creating pre-configured & dynamic templates that are not the completed assemblies there are still many steps required that a DVR wouldn't be a useful setup at this stage of development.  It's an option that's going to require some training sessions, documentation development, etc for my international teams; but if such a feature was available as I described, I wouldn't have to bother with this follow up and training for the masses.

[LukasZygmunt]

Hi @llorden4,

For assembly template,  you can create an iLogic rule which will always change visibility this part to off before saving file. You can do this using event trigger, and you need also remember that you should take BOM structure of this part to Reference. 

I think this is the easiest way. 

If I misunderstood you, maybe you can share some screens, then you explain what you want to hide. 

[omartin]

In drawings, you can assign the part to a layer and have the layer set to not print, but it will still be visible.

But you cant assign parts to layers on a model level, so every drawing that includes the part you would have to always assign it to a layer...you can always write a macro to do it for you however.

[llorden4]

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@omartin wrote:

In drawings, you can assign the part to a layer and have the layer set to not print, but it will still be visible.

But you cant assign parts to layers on a model level, so every drawing that includes the part you would have to always assign it to a layer...you can always write a macro to do it for you however.

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This is basically what I'm looking for, the issue is that drawings are handled by the drafters much farther down the line and I really looking for the ability to turn off the print ability from the part level.  Since these items could pop up in any particular design, pre-configuring some drawings isn't really an option; but you're on the right trail I'm looking for.

[llorden4]

Yes, I get what you're saying; I just don't like the proposed solution.  I know I can set trigger events to run a rule that'll turn visibility on and off.  What it most annoying about your suggestion is every time someone would do a manual auto-save the visibility goes off and then they have to turn them back on again.

I've also picked up on your repeated point of setting the BOM structure to reference, noted it myself in my original post along with mass overrides to zero of things I've already handled.

Presently I can live with the the dashed line approach but I'd also very much like the option to prevent these items from printing on whatever drawing they end up on.

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[marcin_otręba]

Maybe solution will be to create some marking (part can be set as reference or something) then you need to ad add-in or ilogic which will be triggered and check whole assembly (or maybe firs level only) and if such part will occure then automatically will be created view representation (let say print) and then in drawing if you will set rule triggered when saved which will check if reference assembly have such view representation and automatically will change all drawing views representation to print. In addin i am almost sure you can use place view event:

Private WithEvents oUINewDrawingView As UserInputEvents

[llorden4]

That's a whole lot of work, but probably the best approach via iLogic proposed thus far.

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@marcin_otręba wrote:

Maybe solution will be to create some marking (part can be set as reference or something) then you need to ad add-in or ilogic which will be triggered and check whole assembly (or maybe firs level only) and if such part will occure then automatically will be created view representation (let say print) and then in drawing if you will set rule triggered when saved which will check if reference assembly have such view representation and automatically will change all drawing views representation to print. In addin i am almost sure you can use place view event:

Private WithEvents oUINewDrawingView As UserInputEvents

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[marcin_otręba]

There you go. It is base to start.

Both rules should be triggerd when doc is saved.

assembly:

If ThisDoc.Document.SubType ="{E60F81E1-49B3-11D0-93C3-7E0706000000}" Then
Dim ass As AssemblyDocument
Dim cmd As AssemblyComponentDefinition
 ass = ThisApplication.ActiveDocument
 cmd = ass.ComponentDefinition
Dim occ As ComponentOccurrence
Dim ovr As DesignViewRepresentation

For Each occ In cmd.Occurrences

If occ.BOMStructure = BOMStructureEnum.kReferenceBOMStructure Then
Try
 ovr = cmd.RepresentationsManager.DesignViewRepresentations.Item("print")
Catch
 ovr = cmd.RepresentationsManager.DesignViewRepresentations.Add("print")
End Try
ovr.Activate
occ.Visible = False
ass.Save
End If
Next
End If

drawing:

If ThisDoc.Document.SubType = "{BBF9FDF1-52DC-11D0-8C04-0800090BE8EC}" Then
Dim ThisDrawing As DrawingDocument
 ThisDrawing = ThisApplication.ActiveDocument
Dim ass As AssemblyDocument
Dim cmd As AssemblyComponentDefinition
 ass = ThisDrawing.ReferencedDocuments.Item(1)
 cmd = ass.ComponentDefinition

Dim osheet As Sheet
Dim oview As DrawingView
        Dim ovr As DesignViewRepresentation = cmd.RepresentationsManager.DesignViewRepresentations.Item("print")
          If ovr.Name = "print" Then
            For Each osheet In ThisDrawing.Sheets
            For Each oview In osheet.DrawingViews
            oview.SetDesignViewRepresentation ("print")
            Next
            Next
       End If
End If