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Hide and show or layers ?

Hide and show or layers ?

Hide and show or layers ?

(OP)
Hi,
I don't put plane, sketch or others geometry on layers, but I use the command hide or show.
Sincerely I prefer this workflow then activate / deactivate layers, but the problem occurs when I edit the part in assembly, where all plane or sketch are shown again.
I know that on contest edit the reference set goes to 'entire part', but why if I hidden some entities in part, they are show all again ?
If in assembly editing I hide again all planes or sketches, they remain hidden.
Solutions , ideas to avoid to re-hidden geometry entities ?
 

Thank you...

Using NX 8 and TC8.3

RE: Hide and show or layers ?

I suspect that if you go to...

Preferences -> Assemblies...

...you will find that near the top of the dialog the 'Display as Entire Part' option is toggled ON.  If it is, may I suggest that you toggle it OFF and see if this gives you the behavior that you're looking for.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.
 

RE: Hide and show or layers ?

(OP)
Hi John,
I know this setting, the problem is when I edit sketches or planes.
If I edit sketch, 2D entities aren't shown for example end if I edit planes, parent plane is not show.

Thank you...

Using NX 8 and TC8.3

RE: Hide and show or layers ?

Are you using Reference Sets to define exactly what is to be shown at the assembly level, like MODEL ("BDY")?

RE: Hide and show or layers ?

OK, try this.  Go to...

Preferences -> Sketch -> Session Settings

...and check the status of the 'Maintain Hide Status' in the 'Task Environment' section of the dialog.  Make sure that it's NOT toggled ON.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.
 

RE: Hide and show or layers ?

(OP)
Hi MASawtell,
I don't create extra reference set.
I use only 'Model' and 'Entire Part'.
In 'Model' only body/bodies.
I leave NX settings to his out-of-the-box values and let the system take care of things for me.

Thank you...

Using NX 8 and TC8.3

RE: Hide and show or layers ?

(OP)
Hi John, the setting you suggest me is a default in our template as in NX.
This is what happen on edit.
Think a file with 2000 feature where there are lots of planes, sketches, references entities.
I don't use layers, but only show and hide in part.
I use the reference set 'Model' for the component in assembly.
When I edit this part, become 'Entire part' and ALL are visible.
I would like to edit the part in assembly as I'm in the 'Displayed part', so I decide with the command show what I want to show.
Do you use layers or hide & show command ?

Thank you...

Using NX 8 and TC8.3

RE: Hide and show or layers ?

If you have the Assembly Preferences set as I described in my first response above, that is the 'Display as Entire Part' option toggled OFF, then when you set a Component to be the Work Part while leaving the Assembly the Displayed Part (i.e. Working in Context), then the Component's Reference Set will still be Model and your 'hidden' objects will still be hidden.  I just tested this and it works for me.

As for my personal preferences, I prefer working with Hide/Show and NOT using Layers.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.
 

RE: Hide and show or layers ?

John,
With the options you describe, the datums & sketches won't be available unless they are included in the model reference set, or until you switch to entire ref set (at which point everything shows up whether it was hidden or not); unless I am missing something?

RE: Hide and show or layers ?

(OP)
Hi John,
as you, I don't use layer to hide planes, sketches or reference geometry, but I use the hide & show command.
So, how do you do if you have 800 feature in part between planes, sketches or reference geometry that you have hidden in part and you would edit this part in assembly context ?
You will see again all planes, sketches and reference geometry.
What is you workflow ?
Actually I use the CTRL+W to hide planes, sketches and reference geometry again.
I think this is an useless step or I'm missing something ?

Thank you...

Using NX 8 and TC8.3

RE: Hide and show or layers ?

OK, this behavior has always been like this.  If you wish to see the Sketch Curves and Datums you will need to load the Entire Part Reference Set, but than as you've stated, you will see all of the sketches and dataums in the model.  Now there is one thing which is making this less of an issue if you're creating feature where the sketch is 'Internal'.  In that case they will NOT show up when set the Component to be the Work Part (and the Reference Set to be Entire Part) but the sketch will automtically be displayed and selectable when and if you edit it, and it will be removed from the display, even if you're still in the Work Part, when you finish editing the sketch.  But this behavior is only for sketches which are internal to their features.  So if you can make your sketches internal, do so as this will give you something closer to what you're looking for.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.
 

RE: Hide and show or layers ?

(OP)
John,
I know that this behavior has always been like this.
But I'm asking you that you are inside the NX system, if you promote / suggest / use the hide & show as method / workflow, how do you can manipulate in a simple manner file in context that have 800 / 2000 feature (see FIAT or GM or Chrysler file) ?
There are area where NX can improve with a simple option.
Sorry, but will be useful that NX employees use NX to make interesting project not only cube to understand where NX need to be implemented.
It's impossible to add en ER, because is not a limitation, GTAC say to use Layers.

Thank you...

Using NX 8 and TC8.3

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