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NX Part Family vs Solidworks Configuration

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor

 

Hi guys,

 

We are getting into competition against Solidworks with it's Configuration ability.

You can see the below information on Youtube.

 

Creating a configuration

https://www.youtube.com/watch?v=atQ9dCepg6Q 

Using in Assembly

https://www.youtube.com/watch?v=MBsWjPdci04

 

It is a very easy to use tool doing:

 

- Create parts like we do in NX Part Family

- Not necessarily create the parts in the computer..

- When user adds that part into an assembly, he can choose which configuration to use from the table.

- That way the part can be different in two different assemblies but the original part is still the initial version.

 

Much like our Machinery Library.

 

The problem is, with which feature we should offer to our customers?

 

Cem

6 REPLIES

Re: NX Part Family vs Solidworks Configuration

Siemens Phenom Siemens Phenom
Siemens Phenom

Fundamentally, if the set of parts that will be created from the "Parent" are:

 

1) Already known, and

2) Can be described ahead of time in a spreadsheet, and

3) Should never be edited after creation (read-only standard parts)

 

...then I would recommend that the customer use Family of Parts to store the variants and then use the Reusable Component technology available through the Reuse Library to create the simple UI for selection/configuration.

 

Note that ALL THREE criteria above really need to be true for me to steer customers in this direction.  The current Read-Only nature of Part Family Members really limits their usefulness to very standard parts -- which is the driving reality behind #3 above.

 

If the set of parts that will be created from the "Parent" are either:

 

1) NOT already known, or

2) Cannot necessarily all be defined in a spreadsheet, or

3) Need to be editable after creation

 

...then I would recommend steering the customer toward defining the variants in expressions (possibly in conjuntion with an external spreadsheet, on a case-by-case basis) and then using Product Template Studio to create the simple UI for selection/configuration.  

 

Again, note that if ANY of these three are true, I'd steer customers away from a solution based on Part Families.

 

We obviously don't have a 1:1 identical technology as SW Configurations, but we have some pretty good options.  As always, suggestions for improvement are encouraged.  :-)

 

Does that help at all?

Taylor Anderson
NX Product Manager, Knowledge Reuse and NX Design
Tel: +1 (602) 441-0683
taylor.anderson@siemens.com

Re: NX Part Family vs Solidworks Configuration

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor
Of course!

Actually I created a simple part family.
Then opened the main part. Launched PTS Author. Clicked part family refinement but it did not see any family members.
Is there a way to do that?
If there was, possibly selecting which part of that family to be in the assembly after PTS, would be nice.
When I opened PTS Author in NX10 on a main part of a family, I saw 3 motion parts in it.

Cem ALPAY
Yönetici
Üçgen Yazılım Ltd. Şti.
--Iphone'umdan gönderildi--

Re: NX Part Family vs Solidworks Configuration

Siemens Phenom Siemens Phenom
Siemens Phenom

Sounds like you're trying to mix the solutions here...

 

Family of Parts + Reusable Component (KRX) is one option.

 

Parametric Parts + Produt Template Studio (PTS) is the other.

 

In a word, I'm pretty sure that the Part Family Refinement capability inside PTS is not the solution you're looking for.  Man Happy  It's just not a mechanism for doing this kind of creation/configuration/UI for individual parts.

 

Again, IF your situation meets ALL THREE of the criteria for using Part Families, then I'd steer you toward Reusable Components (also called Knowledge-Enabled Components) to create the UI for selecting a family member.  (As you mentioned, like the Machinery Library.)  Docs are here:

 

https://docs.plm.automation.siemens.com/tdoc/nx/10/nx_help/#uid:index_reuselib:id976531

 

And if your situation does NOT meet ALL THREE of the criteria for using Part Families, then I'd steer you toward PTS for the UI creation.  Again, the Docs are here:

 

https://docs.plm.automation.siemens.com/tdoc/nx/10/nx_help/#uid:uid:index_product_template_studio

 

There's also a really good PTS course available on Learning Advantage. Look under "CAD - Intermediate Applications".

 

http://training.plm.automation.siemens.com/mytraining/sp_list.cfm

 

[For the interested observer, the Part Family Refinement capability inside PTS is a specialized tool used in more complex assembly-based Product Templates that contain components that are parametrically selected children of part families.  For more than a decade, it has been possible to have part family members automatically reselected as parametric changes are made to an owning assembly.  The Part Family Refinement control is used to allow a user to manually refine selection of an appropriate family member in the rare cases where the parametric selection scheme set up by the template author was incomplete, and has left more than one valid component that matches the selection criteria.  If parametric selection has not been set up in the template, then this control will not do anything at all.]

 

Does that help?

Taylor Anderson
NX Product Manager, Knowledge Reuse and NX Design
Tel: +1 (602) 441-0683
taylor.anderson@siemens.com

Re: NX Part Family vs Solidworks Configuration

Phenom
Phenom

SolidWorks configurations in assemblies are similar to arrangements in NX.
SolidWorks configurations in parts are similar to part family in NX.
There are similitude but are different.
SolidWorks configuration is a better idea :
1) You can create dynamically or via Excel
2) Can switched rapidly and dynamically in assembly
3) Store in the file only the difference and only the difference is open in the RAM
4) Don't need to store the difference as a different part
5) Can be used as different state in the same part like deformation or pre-machined, etc.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: NX Part Family vs Solidworks Configuration

Valued Contributor
Valued Contributor

cubalibre00 gave a great explation,  I hope Siemens pays attention to it and tries to incorperate this into NX.

Using NX 8.0.3.4

Re: NX Part Family vs Solidworks Configuration

Phenom
Phenom

@aluminum2 wrote:

cubalibre00 gave a great explation,  I hope Siemens pays attention to it and tries to incorperate this into NX.


Without adding enhancement request, Siemens doesn't do nothing.

Change philosophy is a big code reworking that doesn't close a gap.

I'm sure that never will be implemented into NX.

Thank you...

Using NX 11 / RuleDesigner PDM