in isometric view I can not see anything

[mena2001ro]

Hello,

I use NX 7.5 and I have made an assembly drafting. I have already created the drawing views and now I have to insert an isometric view of the assembly. Unfortunatelly, I can't see anything in this view. I have to say that all the layers are visible and selectable.
I'm sure there is a setting, but I don't know where to look.
Can anyone help me?
Thank you!

 

[JohnRBaker]

Select the view, press MB3, select 'Style', open the 'Perspective' tab and hit the button labeled 'Fit Planes to Extents'. And if that doesn't solve the problem, check to see if the 'Perspective' option is toggled ON. If so, try toggling it OFF.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[mena2001ro]

John, thank you for your advice, but it didn't work.
I have finnaly solved the problem toggling "off" the option "Reference" from "View Style" command, "General" tab.
Unfortunately, I really don't understand what this option does... but in this case it worked.
Thanks again!

 

[JohnRBaker]

The 'Reference' view option allows you to turn OFF the display of a drawing view so that when you're working on a large and complex drawing and you need to perform updates and so on, that those views which have been 'referenced' will not slow down these updates. In fact, there is NO reason why you couldn't set all the views to 'Reference' except the one that you're actually working on.

And once you're done adding annotation and creating sections and detail views, adding whatever additional items are needed to your Drawing you can leave as many of the view in this 'Reference' status as you wish since when you 'export' the Drawing, either by plotting/printing it or as a PDF or CGM file, the 'Referenced' views will all be displayed as expected. They only are 'invisible' when working with the Drawing on the screen. This can help you overcome performance issues when all that you need to do is open a drawing to add a few additional items, edit something which may only require access to a couple of drawing views, etc.

Also, years ago, there was a limitation where you could only display on the screen something like 50 active drawing views on a single drawing sheet and so this was a way to allow you to have more than the 50 views on a sheet by setting some of them to 'Reference' status.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[Toost]

An item for the "Features that maybe should be removed in the next release" list ?
- Or do anybody actually use it ?

 

[JohnRBaker]

No, this is actually one of 'features' which we recommend using when you're working on large and complex drawings even if you only have a small number of views since it can help to improve performance significantly if you understand what it does and how it behaves. And while it might be true that it's original implementation was to overcome a hard-limitation (number of active views) which is no longer an issue, the secondary advantages are more than sufficient to keep it on the View Style dialog as a fully supported option.

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

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[mena2001ro]

John, thank you for your explanation, it is very useful. Now I understand what the option "Reference" does and when I should use it.