Product Outline in Drafting

[DipakPatil333]

I have a very large assembly drawing. It takes lot of time to open & update.
I tried using the product outline method. but the views are showing all the curves which it has outlined.
It should show the curves which are applicable to the view.
Can anybody explain how i can do this.
Please see the attachement.

 

[JohnRBaker]

First off, WHAT ATTACHMENT? Second, what version of NX are you running?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[DipakPatil333]

I am using NX8.5

I question is is Prodcut Outline works in drafting mode?
I am able to give dimension, not able to take section view.

Is Product Outline suitable for 3D only?

 

[DipakPatil333]

I am using NX8.5

I question is is Prodcut Outline works in drafting mode?
I am able not to give dimension, not able to take section view.

Is Product Outline suitable for 3D only?

 

[JohnRBaker]

Why would you want to use a 'Product Outline', something which was NEVER intended to work in Drafting, when you ALREADY have 'Smart Lightweight Views' in Drafting, which was designed specifically to address your situation? Are you using 'Smart Lightweight Views' when creating your Drawings? If not, why not?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[DipakPatil333]

Hi thanks for the reply.

I never gone thru this 'Smart Lightweight Views.
Can you please explain me this option in brief or give me some link so i can go thru that.

thanks

 

[JohnRBaker]

It's all covered in the 'What's New' guide (it's the first Topic in the Drafting section of the document).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cubalibre000]

Product Outline can be implemented via ER to use in drafting for situation where you put in drafting very big assembly.
The correspondent solution (Product Outline) is present in SolidWorks form some years ago.

http://www.youtube.com/watch?v=WHfe2RlnFts

http://www.youtube.com/watch?v=vYZw4duM8nI

http://www.youtube.com/watch?v=HudqtnSGUE4

Those are video from SW2009, now SW is on 2014 beta.

So I like your idea/suggestion, but you have to add to Siemens PLM via Enhancement Request.


Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

Since the implementation of 'Smart Lightweight Drafting Views' in NX 8.5, I suspect that any Enhancement Request for something like this will probably not be given much consideration. You can open an ER if you wish, just don't hold your breath.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[uwam2ie]

@John
will Smart Lightweight Views replace the leightweight views from productoutline and facet?
regards

 

[JohnRBaker]

The only thing that 'Smart Lightweight Views' and 'Product Outlines' have in common is that they are both based on using faceted representations. However, 'Smart Lightweight Views' is a Drafting only feature while 'Product Outlines' are used as a sort of spatial 'placeholder' which allows you see the context in which a loaded Component(s) exists in an Assembly even if the rest of the Components of that Assembly are not loaded in the current session.

As for 'Smart Lightweight Views' and the older 'Facet' Drawing views, which we've supported for some time, while the idea is that 'Smart Lightweight Views' can and could eventually make the older 'Facet' views all but obsolete, there are still some significant differences. To start with, the absolute 'lightest weight' (using the least amount of memory and having the fastest update) drawing view that you can create will still be the older style 'Facet' drawing view. However, unlike the new 'Smart Lightweight Views', a 'Facet' view can only be seen with all hidden lines invisible (i.e. no 'dashed' hidden edges), cannot be dimensioned nor have section views created from them. However, they are still useful if all that you're looking for is a simple illustration, such as isometric view placed on a Drawing so that you can show what the part looks like. However, if you want to have the best performance with the least use of memory yet still be able to create associative dimensions, create section and break-out views, show hidden edges as dashed, etc., then the new 'Smart Lightweight Views' is the way to go. Note that you can still use 'Exact' views on Drawing which will still provide the BEST LOOKING rendered views, that is with no jagged or so-called 'facet' effect (i.e. even small circles are smooth) but they are also require the most memory and take the longest time to update when changes are made to the model.

Anyway, I hope that explains a little better the difference between the various 'facet' type representations used in NX and where they are intended to be used and what they offer or not offer in terms of functionality.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[DipakPatil333]

@JohnRBaker,
Thanks for this option. I tried it & it has given me the great results.
But I have one question can we use this option on existing large assembly drawings/views?
I tried with existing drawing views it does not highlight the Smart Lightweight option.

 

[JohnRBaker]

Drawing views have to be CREATED using NX 8.5 or later in order to use the Smart Lightweight option. Views on existing Drawings cannot be updated/converted.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cubalibre000]

John,
which is the solution to add a big assembly, like a tractor in a drawing for documentation ?
Lightweight representation views added in NX8.5 need to be computed to understand which are hidden or not hidden lines, correct ?
Product outline can be a more light representation, like an image, completely computed bu the graphic card.
Please see the video proposed by my previous post and tell me if is good idea to be implemented in the product outline.
This SolidWorks speedpak is used to add big assembly in drafting.

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

If all you want is an extremely LIGHTWIEGHT 'image' on your drawing, then simple get your display to look like what you want in Modeling. Do an...

Export -> <PNG..., JPEG..., TIFF...>

...and then with your Drawing displayed, use...

Insert -> Image...

...to place this 'image' on your drawing.

That will be the absolute 'lightest' view that you can possibly create on a Drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cubalibre000]

John,
this solution is very extreme. If you change the tractor, the image doesn't update.
SpeedPak in SolidWorks is light like an image, but update itself if the assembly change.

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

Sorry, I've given you ALL the options that we now support. If you think they are inadequate, feel free to call GTAC and have them open an ER.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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