Reference lines of part in higher assembly - can I turn them off?

[adam.krzyzakMEMPJ]

I have a assembly . In this assembly, I set one part as reference. In the drawing of the assembly, this part displays as reference - dashed lines, just as I wanted.

However, this assembly is in a higher assembly. In the drawing of this higher assembly, this part is still set as reference and the lines of this part display dashed. Is it possible to change this? I would like all lines to be as default in this higher assembly.

[jtylerbc]

Yes, but it will affect all reference parts, not just this one.  That may be okay, or could be a problem, depending on what you want.

Edit the view, and in the 'Drawing View" dialog box, go to the Model State tab.  Set the "Display Style" as desired.  It sounds like it would be Edges as Part, based on my understanding of what you want,

[blandb]

If its just the view you are editing of the higher level, I believe "as parts" will work. That shouldn't change lower level drawings where this component is referenced because the view for those drawings are "as reference".

[jtylerbc]

@blandb, that is correct, but isn't exactly what I meant.  I didn't state the issue I was really referring to very clearly.

To clarify, I meant that in the view you are actually changing the setting for, you can't display some parts "As Reference" and some "As Part".  It won't affect the display in other drawings, or even other views on the same drawing, but changing this setting will affect all reference parts in that view.

[Frederick_Law]

You might need ModelState.

How did you set the part to reference?

In assembly BOM Structure -> Reference?

Or in the part's Document Setting -> Bill of Material?

Do you want the part to show in BOM in higher assembly?

Referenced part will not show in BOM.

If it changed to Normal, it will show in BOM/Partlist.  Is that what you want?

As other said, you can change setting in drawing view without changing the part to Normal.

[johnsonshiue]

Hi Adam,

I assume you would like this reference part to be shown as a regular part in the top-level assembly, right? You could edit the drawing view -> Model -> Reference Data -> select "Display as Part."

Please note that this only applies to the drawing view. The part instance will still be deducted in the PartsList.

If you want it to be a regular part display-wise and PartsList-wise, indeed you will need to use Model State. Open the assembly hosting the part and create a non-Primary Model State. Change the part instance BOM structure from Referenced to Default (Normal). Any higher assembly will need to have a non-Primary Model State in order to persist the change in BOM structure at the lower level.

Many thanks!