i want reference part hidden line to show up hidden

[ferrisb]

Any way to do this?

INV 2009

[mcgyvr]

I think this is what you are asking for....edit base view, model state tab, set Reference data line style to "as reference parts"

Now reference parts will show as hidden lines. Default is "as reference parts" so you changed it at some time.

[ferrisb]

Thanks for the reply.

What I'm actually looking for is...

Reference part object lines to look like (x)

Reference part hidden lines to look like (y)

[mcgyvr]

As long as you are okay with ref part hidden lines being the same as a regular part hidden line you can change the linetype of the reference part object lines to whatever you want in the style/standard editor/object defaults

[ferrisb]

That's exactly what I want concerning the hidden lines.

I want hidden lines of refferenced parts that look like other hidden lines.

However, hidden lines are continuious, pahntom, or whatever I set the refference lintype to.

The hidden line of the refferenced part look the same as the object line of the reference part still...

or have I missed something?

is there not a hidden refference line and an object refference line?

[mcgyvr]

Hidden lines are hidden lines no matter if the part is reference or not. There is not a specific object type for "reference part hidden lines"

Reference part (non-hidden/regular) lines can be set to whatever line style you want. These are defined in the object defaults. Find the "Object Type" of "Reference Part Edge" and set it to what you want.

Just make sure your base view is set to display reference parts as reference parts or it will be modified to regular part line type. (like I talked about in my first response to your topic)

[ferrisb]

Hidden lines are showing up as solid here.  inv 2009.

Yes, base view is set to show refference as refference.

Sorry I can't post a better example, working on proprietary stuff here.

When I highlight the edge or part in question the hidden lines show dashed, solid(yellow) hidden (red)

When not highlighted everything appears solid.

[mcgyvr]

Can't tell crap really from your picture. Would have taken you 2 seconds to create a new assembly of non-proprietary information to show the issue... But are you sure you don't have 2 parts on top of each other.. One set to reference and one not?

[ferrisb]

Sorry for the shotty example...

It seems some lines that are from a ref part are not even showing up... (left)

If I change it back to default, it looks fine. (right)

I tried setting ref from BOM and properties, no dice.

[ferrisb]

idw incoming.

[ferrisb]

Would help if I put these under the correct posting : )

still miss the ftp site...

Edited by
Discussion_Admin

[mcgyvr]

In your styles you have the "Reference Part Edge" object type set to use the D-equipment layer which is set as a continuous line type.

[ferrisb]

Yes,

This is what i want reference parts object lines to look like.

I still want their hidden lines to be hidden.

trying a layer work around for acad conversion.

using a ref part to assign objects to a certain layer.

[mcgyvr · Accepted solution]

Ok sorry now I finally understand what you are asking.. The ONLY way to achieve what you want (ref part non-hidden lines being continuous and ref part hidden lines being dashed) is to manually edit the base view and go to the model state tab and select "As parts" for reference data. Then and only then can ref parts have 2 line styles.

By default "as reference parts" is checked (forced) and you cannot change that in your template and have it stay persistant.

When it is set to "as reference parts" any reference parts can ONLY have 1 line style that can be assigned to them. Visible or hidden sections will always display the same line type.

[ferrisb]

Thanks for all the help!

Was worth a shot!

[cwhetten]

I'm having a hard time understanding what exactly you want to do, but perhaps this will help?

The above settings will make your reference parts look exactly like every other part (except in shaded views, reference parts will not be shaded).

Hope this helps.

-cwhetten

[mcgyvr]

Yep but he didn't want to set that manually each time he creates a drawing.He ALWAYS wants ref part regular lines to be continuous and their hidden lines to be hidden line style.

If the Inventor styles included an object default for reference part hidden lines or Autodesk allowed setting/changing the default values for those settings in the base view model state tab, or if hidden lines were hidden lines no matter if its a ref part or not the problem would be solved. Now its just a manual workaround everytime he creates a drawing.