Reference parts show heavy lines

[acorn77]

A seemingly nice feature turns into a hassle when in a
drawing. I can go to properties ,then occurrence and set the
value to reference for parts I do not want showing up in
the BOM. But then those parts show up in the assembly drawing as heavy thick lines. Is there a fix for this other that
showing contents and then shutting of visibility entirely?

Thanks Don

[Anonymous]

Change the line weight for what ever layer your reference edges are landing
on. This should be set up permanently in your Styles Library.

[acorn77]

Thank You Dave,
I found them as phantom lines not reference lines because they were the thickest. Also they were set to dashed & I changed them to continuos. I hope they are not used elsewhere to mess something else up.
Don

[kgrunawalt]

Another strategy: If you have a part that you do not want to appear in any BOM/part list, you can set the part's BOM Structure (Document Settings/BOM) to Phantom or Reference. What is the difference? If you set the BOM Structure to Phantom, the part will appear unchanged in drawing views. This approach will work if:

a) The document is a part and not an assembly. Phantom assemblies will also not appear in a structured bom, but their children are promoted to the assembly's level. You may not want this.

b) The document should never appear in any part list. Changing the document setting instead of using the BOM Structure override on an instance of the part will affect all BOM views that include that part. You cannot set an instance of a part to Phantom. You can only override the part document's BOM Structure by making the instance Reference.

Summary: you can remove a part from all part lists/BOM views without affecting drawing views by setting the BOM Structure to Phantom in the part's document settings dialog.

Katrin Grunawalt (Autodesk)

[Anonymous]

View your Object Defaults to see where else they are used. You should
probably leave them as dashed. You can set them to display as continuous at
the view level by rmb on the view, Edit, Options tab. You can change the
line style of the reference data there. This gives you different options for
different situations. (I have a layer called "Reference" with a Dashed line
weight of .007)


> I found them as phantom lines not reference
lines because they were the thickest. Also they were set to dashed & I
changed them to continuos. I hope they are not used elsewhere to mess
something else up.
Don