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NX Simplify Assembly Function Large Assembly Management

Genius
Genius

Mainly for Siemens staff or anyone in the know...

Is the Simplify Assembly function still a mainstream utility for managing large assemblies in NX10?

Given other CAD systems (Creo, Solidworks, Catia, etc.) have lightweight and complexity reduction functions I still see they all utilize "enveloped" style components for use at the next assembly just as NX does with Simplify Assembly. So it appears other CAD tools still find it a necessary function to have, is that the future case for NX as well?

 

The way I see the Simplify Assembly function would be used is as follows:

1) Build complex component model with many parts

2) Create a linked Simplify Assembly feature which is stored in a special Reference Set with in the complete component assembly that hides all internals and gives an accurate external representation of the component (Lets call that reference set "Envelope")

3) Assemble said component at Next (Top) assembly.

4) Set Reference Set load order to have "Envelope" followed up with "Model" and so on...

5) When loading the Top Assembly it will load the Simplifed versions of the components using the Envelope reference sets.

 

Is this what is still envisioned using NX10 for extreme Large Assembly model management for reduced RAM pull and faster model load times, along with Lightweight representations?

 

Or is Siemens going away from the Simplify Assembly function?

Or is it worth using, as stated above, meaning does it save Load time and RAM pull?

 

Thanks!

17 REPLIES 17

Re: NX Simplify Assembly Function Large Assembly Management

Genius
Genius

Hello,

 

what really helps with LARGE assemblies is the "representations" feature. You can either use it out of the box (advanced assembly license required) or with the help of several tools like http://neoapps.de/en/nx-representation-en/ or similar (I am not connected to that company)

 

regards,

Josch

Re: NX Simplify Assembly Function Large Assembly Management

Genius
Genius

Josch,

Have you found that using Representations (NX 10 Help Link on Representations) is all that is required in any large assembly without the need for any further simplification of the model?

 

Have you ever had to use the Simplify Assembly function to achieve a manageable assembly before or after using the Representations?

 

Thanks!

Re: NX Simplify Assembly Function Large Assembly Management

Genius
Genius

I guess from the lack of response to this post I assume that most folks don't use the Simplify Assembly function? I would think that the ship building community would probably use this the most often to reduce memory usage and load times given how large a ship top assembly would be.

Re: NX Simplify Assembly Function Large Assembly Management

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

Hi Corey, I have discovered this post only now, I think the workflow you suggest (Simplify Assembly and dedicated Ref Set) is really a precious tip! I am working both with large building models and boats and this solves many problems. I also use another 'structure':

Simplify Assembly feature in each 'top level' Assembly; lower level components all closed. 'Above-all' level  Assembly loading all the said 'top level assembly' containing Simplify Assm feature.

In this way I need to load a much reduced number of components. Loading is really faster, and drafting also.

I also use Simplify Assembly features without really 'simplify': I skip the 'leak check' option and I just 'sum up' in a single feature only the bodies I want to see in a particular contest: this may seem silly, but again I can see what I need loading only one file instead of all the components.

I think that people who only use Lightweight representations don't have the most critical problem that we have in shipbuilding and architecture, that is being able to 'represent' things at different scale (the more the scale increase, the less detail you need: at 1:100 I cannot use a model with all the details of a 1:1).

Laura

 

 

 

Re: NX Simplify Assembly Function Large Assembly Management

Genius
Genius
Thank you for the reply Laura! That's awesome to hear someone else sees the use of the Simplify Assembly function in the same and similar fashions as I use it for. I also almost always skip the leak check part of the function and use it exactly the same way where I select only the things I need, unite them, and cut (extrude) away any internals I can clean out. I've found the sealing and closing up of the component is usually very time consuming and it really doesn't gain that much more than just doing the simple selection and uniting that you also do.

Thanks again for the reply!

Re: NX Simplify Assembly Function Large Assembly Management

Pioneer
Pioneer

For step 2.) Create a linked Simplify Assembly feature which is stored in a special Reference Set with in the complete component assembly that hides all internals and gives an accurate external representation of the component (Lets call that reference set "Envelope")

 

How do you store the simplified assembly in a special reference set? I know how to create a new reference set, but it will not allow me to select the "Simplify Assembly" feature I created.

Re: NX Simplify Assembly Function Large Assembly Management

Genius
Genius

Unfortunately the reference set won't accept the Simplify Assembly feature directly as a click on the feature.

The way I get the geometry within the Simplify Assembly into the other reference set is I "Show all" to ensure all the bodies associated with the Simplify Assembly are shown.

2019-02-01_18-41-28.png

Then I hide everything (datums and components especially) except bodies. 

2019-02-01_18-31-04.png

 

Once those are hidden go to the reference set function and box select the items left on the screen.

2019-02-01_18-33-53.png    2019-02-01_18-34-11.png

 

There's also another way, but only in NX versions 12.0.2 or later where they corrected a bug. You'll notice the reference set I have selected has the word "Simplified" in front of the Reference Set name. In the customer defaults there is a Simplified Automated Reference Set. This is for when you use a Wrap Assembly, Linked Exterior, or Simplify Assembly (only in NX 12.0.2 or later) the features automatically get added to the named reference set in that customer default. If the reference set doesn't exist yet the default simplified reference set automatically creates it. Before NX version 12.0.2 only the Wrap Assembly and Linked Exterior get added, but Siemens corrected that in 12.0.2 so the Simplify Assembly is also included.

 

2019-02-01_18-36-43.png2019-02-01_18-37-14.png

Re: NX Simplify Assembly Function Large Assembly Management

Phenom
Phenom

Hi,

my opinion is that Siemens PLM need to implement a new way to open big assembly. The new way seam to be available starting NX12.0.2 with TC, but this has some limitations.

I would like no limitations and work also on native.

I would like to test this new implementation respect what SolidWorks does from some years ago.

NX Simplify Assembly is a time consuming, during creation and in case the assembly change. Lot of work.

Thank you...

Using NX1859
RuleDesigner PDM

Re: NX Simplify Assembly Function Large Assembly Management

Genius
Genius

I agree having to have the limitation of being attached to Teamcenter for the new assembly loading option is unfortunate. I know they are looking into ways to processing the data even in native format, but with the Minimal loading they are taking advantage of the server caching as a way to load the data while you are able to still interact with it during the loading. I'm not sure if they can do something on the machine to mimic that so it also works in native, but I know it is a request made by many.

 

When you mention Solidworks are you talking about the SpeedPak functionality?

I've utilized Solidworks in regards to their SpeedPak assembly management and it even has some very annoying issues because, just like NX, it's trading one thing for another to allow for quicker display and loading. This in turn causes limitation like referencing items in the model and drawing, creating BOM's, and selecting specific geometry.

http://help.solidworks.com/2019/english/SolidWorks/sldworks/c_SpeedPak_OH.htm

 

NX Simplify Assembly is definitely an old function that needs updating and I have heard of a project they are working on replacing it with a new designed function (I'm assuming the old will remain for data management) that will provide more automation and smarter simplification tools. I have no idea if or when it will be released, but they are definitely spending time on that future functionality.

 

When we use NX Simplify Assembly the time consuming part is most definitely an issue so you have to remember to only spend the time in the areas that benefits the simplification directly.

For example only include the components you need to represent the complete external assembly. Unite those items and maybe use a single extrude to remove what internals are left over. I would never spend any time trying to close out a model for the Leak Test.

Depending on the model, the time and effort it takes to close it out is not worth the load time and memory saved by having a completely solid internal. Once the leak function is ignored from ever being used the time consuming part goes down dramatically.

For updating the Simplify Assembly it again takes a bit of NX finesse. The function will only update if the Delay Updates is turned off. If you're working on assembly to update it's simplification I would only load that one assembly. Then I would disable the Delay and allow the Simplify Assembly to regenerate. It'll either show with a Green check or a red X. If it's red you have edit the function and I would recommend going past the first window to allow for any missing bodies (typically due to component deletion) to be deleted then return to the first window and add or remove what's needed. Just some pointers I've learned from using the function over the years. Fingers crossed a new function is on the horizon.