Should one model contain multiple parts and drawings. ..? (NX6)

[JohnFox]

Hi,
I have happily created a model that consists of an object with multiple parts (in this instance a working tool).
How should I proceed in relation to making engineering drawings for each part? I have tried to show or hide each part in the modeling area and then create a new drafing sheet for each subsequent part but this did not work to well as the drawings always wanted to update to the present modelling view. How do people manage this situation?

Should I be modelling my object and then creating an assembly (i.e.wave linking the parts into it?) - does each assembly member have its own drawing?

Can I get multiple different drawings in the same .prt or should I be looking to split the part into its constituent parts after creatation and have one drawing for each part?

Many thanks for any advice!

cheers,
JohnFox

 

[JohnRBaker]

Technically there's nothing stopping you from doing anything. That's one of the 'charms' of NX, not that that makes life any easier for anyone ;-)

First a couple of questions, these individual 'parts', were they created in a manner which referenced each other? That is, does one part depend on some edge or face of another part? If not, then you can make an assembly out of what you have pretty easily. Just go into...

Assemblies -> Components -> Create New Component...

...assign a name to a component, select a body you wish to assign to that component (be sure that the 'Add Defining Objects' and 'Delete Original Objects' options are toggled ON). Repeat for each 'part' in your original part file until you've 'converted' all of your 'parts' into Components. Now do a 'Save All' and you got an assembly and separate files for each Component. Now, open as the displayed part each component and then do a File New selecting a Drawing template and you've got the start of a Master Model drawing. Repeat this for each component and you will have drawings for each component (you'll probably want to also make drawing of the assembly file itself.

Now if you have been referencing one 'part' to another, if you don't care about the models being parametric, you could remove all the parametrics from all the 'parts' and then follow the process described above. But if you wish to keep everything parametric and associative, it's going to be a bit more tricky as you will have to decide whether you really want an assembly or not.

If not, what I might suggest is that you create a Reference Set for each 'part' and then open individual drawing files adding as a component, but using a different Reference Set each time, your original part file. Now this will result in multiple Drawing files all referencing the same Master Model. Now this may not be ideal, but it will work and it allows you to maintain, without a lot of extra work, all of the 'inter-part' relationships between your 'parts'.

Now as for trying to do all of this inside of just part, that can be done, but it will require you to do a lot of organizing with things like layers so that you could create multiple drawings each referencing a single 'part'.

Anyway, once you sort this all out, we would recommend that you take what you've learned and try to use a more traditional approach to deigning your products, working in a bottoms-up approach, if for no other reason than that often is the most efficient, particularly if you have a lot of parts which can be reused from one project to another or you have a lot standard (purchased) parts.

I hope that was clear. If not, I'll try and answer any specific question that you might have. Also, others may some ideas as well. Like is said, the good news is that NX has enough flexibility to do almost anything in any manner they you wish, but there are some approaches which are more productive than others and you should review all of them before you start another major effort.

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.org/museum/

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

 

[hudson888]

The shorter answer is you can if you wish, but not if I had anything to do with it. The more elegant method that reflects the features of NX as they have been designed to be used is called the master model approach and involves the creation of assemblies and components each with their own drawings all off which are in separate files.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[SiW979]

I agree with Hudson, 1 single component per drawing, this is especially true if you are going to use Teamcenter for your structuring (BOMS)Even if we have the simplest welded assembly of two single but different components, we will do three individual models and drawings - 1 for each single piece and 1 for the welded assembly.

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[JohnFox]

Hi Guys,
thanks for the great answers! I will work through with the master model approach.

cheers,
JohnFox