Can an assembly be stripped of parameters...

[3dr]

with out Stepping it out??? I'm thinking like a "delete all parameters" command. I've got one thats become a burden at the documentation stage... i'm wishing I had tried te "historyless" method at this point. Maybe it would have served me better at the end.

TIA

Dave

 

[SiW979]

You can use Edit --> Feature --> Remove parameters

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...

 

[3dr]

That only works for content within a componet. I've got a large ass'y and want to strip all the componets down at once.

 

[jerry1423]

Are you talking about removing the mating conditions?

You mentioned not doing a STEP export, but you can do a parasolid export.

 

[cowski]

What type of burden are you running into? Slow visualization (rotate, pan, etc), slow drawing view creation/update?

Unless all of your components are fully loaded, I don't think history free mode would have helped (or removing parameters now is going to help).

 

[3dr]

I meant all internal part parameters used to build the solids. I'de like to be able to use a "remove parameters" command like the one JCBCad offered but do it external of the target part.

My slow down appears to be general "bogging down" of the whole design. I copy and paste attributes for BOM content between parts and save them as the actual detail no. Ex: 001, 002 , 003 etc...

The whole process is just terribly slow. Most of what I do in the end requires no mating, sketches etc... it's automtive stamping tools.

Dave

 

[jerry1423]

If I was you I would do a parasolid export then import that parasolid into whatever file you want to, including the one that you are working in. If you do that then you can close the parts in the assembly tree.

 

[SiW979]

Alternatively try wave linking the whole assembly into another file that way you retain associativity which may be useful to you in the future. If it isn't an issue, simply break the link then perform an edit > feature > remove parameter to ensure that all the resulting solids are as "light" as possible.


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...

 

[ewh]

I have approached this similar to what Simon recommends: Insert -> Associative Copy -> Wave Geometry Linker and select all of the components. Then Edit -> Feature -> Remove Parameters and select all of your wave linked geometry.
At this point you will have two bodies for each item; the associative component and the "dumb" solid. If you really don't want any parameters, just delete the components.

While this method works in theory, I have had to export and re-import parasolids in the past a couple of times to truly remove all parameters tied to the parent part (lofted surfaces that just didn't want to give up their history). I haven't tried this method on these parts since NX4, so this problem may be history.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[hudson888]

Dave,

Your situation begs the question why do you want to remove the parameters? If it is just assembly performance issues there are many fine tools for working with lightweight data that could satisfy your needs given they we're not aware or your current motivation.

Some of the above sound like they'd dump all the geometry into a single part file in which case, File>Export>Part, tick on select "All Objects" and "Remove parameters". If your assembly is small enough that the system can cope with doing this you'll have what seems to me the identical result, but with less work.

Alternatively if the assembly is much larger then you really need to preserve something like its structure for sheer performance related reasons, or you may just want to. So I'd probably take the Parasolid route in that case. Failing that you're welcome to try STEP if you're data is simple and unlikely to be degraded as part of the translation process.

The method of wave linking and then breaking the links would in my view be workable though extremely tedious. On some levels if you have to manually remove parameters for whatever reason then you might as well clone the assembly then go about the process of removing the parameters of all the solids in each of the component parts files equally manually!

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[potrero]

In addition to File>Export>Parasolid, you can do File>Export>Part, then configure the parameters to remove parameters.

 

[ewh]

I knew this question sounded familiar; John Baker gave an eloquent solution here -> thread561-250808

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[cowski]

I mostly understand the desire to remove parameters from parts in a large assembly and I understand the methods given to do so. However, I'm still a bit confused about this part:

I copy and paste attributes for BOM content between parts and save them as the actual detail no. Ex: 001, 002 , 003 etc...

If you condense the assembly down to 1 file full of parasolids, won't you lose the individual file/part attributes?

 

[3dr]

Yes I would Cowski! So most of these thoughtful reccomendations don't serve my need with out a negative. I do use componet attributes in my BOM and need to preserve that data.

I lived with design issues I had and shipped the job. All behind me now but I got a lot of responses on this and I appreciate them all.

The only thing that sounds attractive to me for the future at this point is the light weight recommendation. I've never used it and don't know what the potential is for performance gains.

Can anyone speak to that??? I do a fair amount of wave linking to make edits easier during the design process. Move a part and all the mating features in other parts go with it. But at the end of the job all those links mean nothing and get broken when the Ass'y structures are settled.

Can this kind of intelligence be used while in lightweight mode?

TIA

Dave

 

[hudson888]

3dr

You won't loose parameters or attributes in using lightweight geometry. In fact it would seem almost surprising that it wouldn't already exist in many of you models. It is the contents of the REP or FACET reference set so you access it at the assembly level by swapping reference sets. Many systems are set up by default to create these reference sets.

Alternatively if you don't already have these reference sets containing the faceted representations you may occasionally have to create them manually which can be done albeit that you possibly need an Advanced Assemblies license to complete the task.

In terms of taking advantage of it for performance reasons the things to do are to turn on partial loading in your load options, preferably before you open any geometry. Also set your preferred reference sets under the load options settings to REP or FACET depending on your site standards.

That it the potted version about which you may hopefully find any further detail you need after a brief search of the documentation.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

You might as well start getting used to lightweight since that will be the default in NX 7.5 (granted, it can be overridden by the user, but I suggest you give it a try before making any rash moves) and it's being done without depending on Reference Sets which means that it will be even more ubiquitous than what it can be today.

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.