Visible In View or Layer Control

[JPM73]

Hi UG Users,

I have a part that has an handful of layers in it. When I go to the LAYERS SETTINGS options make a specific layer & "Selectable" or "Invisible", my entities on that specific layer does not shut off.

The only way to make these entities "invisible" is to go to the VISIBLE IN VIEW option & make that layer "invisible", which is annoying. This issues seems to be file specific.

Is there a toggle option somewhere so that my LAYER SETTING options will work as they should - Meaning when I make a layer "invisible", it will become invisible, without having to go to the VISIBLE IN VIEW option to make invisible?

Thanks

Jason,
CTQ Engineering
Technical Team Leader
GE Product Definition Designer

 

[JohnRBaker]

Are you talking about components in an assembly being on different layers? If so, don't use Visible in View, just use Hide in View as that is now the preferred approach.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[phillpd]

From the Visible In View dialog, the Reset to Global option can usually remedy this situation.

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[jackley]

This is one of my biggest pet-peeves. An ex-coworker of mine used to do this all the time. How annoying.

IMO, visible in view should only be used on the drawing side.

Justin Ackley
Designer

 

[hudson888]

Jason,

Sounds like you may be a bit new to NX and/or may not be used to using layers. Excuse me for mentioning that because what I'm about to explain may seem condescending to an experienced user and I don't wish to offend. If this isn't for you then other users may benefit...

The common beginner's mistake is that the work layer can't be made invisible under ordinary circumstances. If you make another layer your work layer then you can use selectable and invisible as toggles to turn layers on and off. The other available setting "visible only" is less frequently used.

If somebody else has set visible in view in model space, please find them and punish them on behalf of NX users everywhere. Do as Phil said and reset the view to global, you may need to check out other views in the same model to ensure to expunge this plague upon your house. In many cases the views most affected will be saved views which will have generic names. Try swapping to one of TOP, FRONT etc this is often all that is required.

Go into the layer dialog and look at the information listing. Some people get confused after components are added to certain layers while their entities live on other layers. John mentioned this earlier. People don't read the settings when they add components, if you were on layer 1 in an empty assembly and you added a component with a solid on layer 2 and a sheet on layer 3 then your assembly would have one object on each of the first three layers. The component is on layer 1, but you will only see geometry on layer 2 or layer 3 since the component entity on layer 1 is not a geometric object. This isn't necessarily bad practice just something users need to come to terms with. There are other options with different implications and effects of reference sets that also come into play. I can't explain all of these but a component will be hard to see in the reference set is set to empty for example.

Other sources of confusion can be groups which contain no objects and blanked, (latterly also called hidden), entities. Try running a part clean-up to ensure there are fewer artifacts left over from earlier poor housekeeping.

About another thing that John mentioned; turn on the view names in modeling because exploded views are, if the default convention is followed, named as such. In an exploded view you have an extra way to hide components that again is really only meant to be used for drafting purposes. You can show or hide a component in an exploded view and latterly create this on the fly or by means of editing any view on a drawing. The fact remains that in earlier versions you set this up using exploded views in modeling prior to adding those views to the drawing. If you use exploded views you'll seen realize interacting with them in modeling is pretty much part and parcel of what you need to do. Some people may be working in ways that either inadvertently confuse their colleagues or have developed methods that really represent an unintended method or misuse of the system. However if the last thing that the previous user did was to create an explosion and hide some components then it wouldn't be unusual to save to file with that view displayed, meaning that if the next person opening the file knows little or nothing about exploded views they'll probably be a bit thrown by it.

Please get back as to what worked or if you still have no luck.

Cheers

Hudson