Loading NX5 part on NX4 - Doesn't Work Pls Help 2

[Willzville]

My client cant open my NX5 parts on his NX4 software. I want the file to remain in NX format and not export it to anything else.

How do I allow an NX5 file to be opened on NX4. I've taken all the feature (e.g. black to grey grad background, etc) that NX4 doesn't have and it still won't work.

 

[hudson888]

Will

The best way would be to send a parasolid or if it is and assembly then via step214. NX is NOT backwards compatible.

Do consider checking how much of the model was actually saved in NX-5 if you have upgraded recently you may find that some of your components remain unchanged and can still be opened in earlier versions of NX.

Best Regards

Hudson

 

[argeportal]

You can also export your NX5 files as NX part file from menu "File-Export-Part" . Exported part files can be opened in any version of NX.

Regards,
Gokhan

 

[hudson888]

Will,

I don't know what Gokhan is referring to but as far as it can be literally interpreted what he has posted is simply and unfortunately not true.


Gokhan,
If you can prove to me that this is true then please thrill me with it. I'd love if it were the case but for the moment I don't know of any interpretation that fits.

Best Regards

Hudson

 

[1wise]

Will,
Hudson is correct. NX is NOT BACKWARDS COMPATIBLE if you want to keep your file as an NX5 your client would need to upgrade or you will need to "export" your file into a different format.

 

[joycejo]

That is true you cannot export a part to a earlier version. NX is NOT backwards compatible. You can export a parasolid to an earlier version V17.0 for NX4 and then open the parasolid file. You will loose all the parameters though :-(

John Joyce
Tata Technologies iKS
1675 Larimer St.
Denver, CO

http://www.myigetit.com

 

[jerry1423]

My best tip would be to contact Unigraphics to see if there is a way for them to transfer an NX5 part to NX4. If you just need the solid model then just import their parasolid file (as mentioned above).

As long as I have been on Unigraphics (20 years) the ability for you to be on the same version as your customers/suppliers has always been a concern - you need to communicate well with them.

You may still have NX4 on your computer and not realize it - if that is the case then open it with that.

 

[ewh]

I have to agree with the others. Short of you recreating your parts on NX4, your customer will either have to upgrade or accept an unparameterized model such as parasolid. This is one of the pitfalls of upgrading ahead of your customer base.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[cbrn]

Hi,
this topic has been already discussed in a -very long- way some time ago. NX is definitely not backward-compatible and probably never will be (it's a pity, but...).

Regards

 

[ewh]

(my favorite)

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[hudson888]

Oh now come on its not necessarily a deadhorse

According to the teaser NX-6 will enable you to change almost anything even if you don't have parameters. Not that they won't be good to have and/or used. But still it may be the case that you don't get to degrade your data as far as you may have done in the past if you have more tools to work with dumb solids etc.

Regards

Hudson

 

[ewh]

Good point, Hudson, but NX6 isn't going to solve this problem, at least not until you are able to open NX7 and above in it, and you still have the issue of customers who don't upgrade. In my opinion, the backward compatibility question is still a dead horse. There may be a solution in the future, but we aren't there yet.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

Please don't start any rumors. The is NOTHING in NX 6 that will address backward compatibility, period! And there are no plans to do anything in that area either as there is little to be gained for an effort that would be monumental to achieve.

The only thing that NX 6 brings to this issue is that, like each release of NX over the past several years, there has been our continued investment in making it easier to work with data from other systems, or what in the industry is called 'multi-CAD' support. It's a fact of life when dealing with OEM, vendor, supplier situations that you are going to have different companies with different systems sharing data so these system have to be able to both coexist and accommodate that. Now to the extent that it will make it easier to edit and modify models from a 'foreign' system, and in the case of CAD software, to an older version, a file created in a newer version might as well be from a foreign system, then YES, some of the technology being introduced with NX 6 will make it easier to recover and reuse data involved in a 'downward' transfer, but only because we improved the ability to handle ANY foreign data, not just because we implemented some sort of downward compatibility feature. Remember true downward compatibility implies that not only does an older version of the code recognize the contents of the newer model, but would also preserve it so that it could theoretically make a 'round-trip' with NO lose of data or integrity, something that would be virtually impossible to implement at any R&D cost.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

John,

All I said was that the new tools kind of meant that losing the parameters was less of a problem. No idea what ewh meant I just supposed that he misunderstood what it was or hadn't yet seen the video and wasn't quite catching my inference.

There is no such rumor that I'm aware of. And I don't intend to start one. I do however wish to put forward a modest observation about the dead horse in question.

The only functionality that I would like to see that may be do-able at a much lower cost, is the ability to open files and assemblies as un-parametric data in an older version on the fly and locked for editing once filed in the newer version. You have to have the requisite warnings but no attempt to reproduce data integrity etc. I say this because there is already interoperability between NX and other systems so that to my mind having to actually use a translator to even access data from one version to the next is a fairly unpalatable prospect.

I don't see that the machining guy has to change my model nor any other downstream user. If they choose to take their own copy and modify it then that should be possible as if a translator had been used and the parameters lost in that process. At some stage some reasonable compromise might be possible without great drama.

See the bitter pill to swallow comes when you have an assembly where either only one part is affected. Or worse you need to send an assembly back with it's structure. parasolid would be the least degradation of the data but doesn't do assemblies, where as Step does but it renders imperfect solids in some cases.

best regards

Hudson

 

[ewh]

Sorry, don't want to start any silly rumors.
My response was refering to the OP's desire to keep the part as NX format, and I assumed he meant as a parametric file with the part history and everything (otherwise he wouldn't have a problem, would he?).
I have NO expectations of complete downward compatibility (as described by John), thus the horse.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[grab1]

Just a thought, but have you tried JT. I'm told this is the way things are going !!!

 

[hudson888]

Grab,

What happens with JT files is that they are exported and can be maintained up to date as such from NX for use with separate viewing software. JT2GO, Vis-View or Teamcenter Visualization, all versions of much the same thing with various levels of sophistication and they go by a few different names I think in slightly different guises so that I'm never quite sure what to call them. Anyhow they create these files which become can work as assemblies. So far good point it has possibilities.

You can open both file and assemblies in NX-5 and indeed in NX-4 from output made with NX-5. However there are some serious limitations firstly if it is an assembly that you're opening then the assembly structure is re-created with kind of a double level for each part having two items in the ant. These can be used and saved as part files if needs be as I'll explain. If you open NX-5 output in NX-4 then the names come out with appended a few extra characters that also don't appear in the original and so aren't quite right. So as far as exporting and importing the assembly structure JT is slightly inferior to STEP214.

Now as regards the actual geometrical data, the files are smaller than Parasolid exports, which is slightly odd since they eventually contain approximately the same thing. I say eventually because the JT data initially imports a faceted version of the models, but you can go into the file properties and extract the geometry to what then results in a unparameterized bodies. The data once extracted seems to be every bit as good as a Parasolid file. While I have seen curve sections exported into JT files used in teamcenter I've not yet discovered how it can be done or whether it can help you get those curves via the JT file back into a previous version of NX. Certainly it is surprising that the data can be extracted so successfully from a smaller file, but if working in an assembly each component has to be done individually, and the extraction is a fairly slow process.

So there you have it not a bad idea, but no parameters certainly no drawings, and few if any entities in fact other than the solids. But better quality data than STEP214, and something of an assembly which if not quite right is certainly not wrong at least.

Because it is a separate file there are still parallels with any other translator, but it is certainly a method I would consider using and perhaps if some of my gaps about the whys and wherefores of curves and other entities can be addressed or responded to here then it has potential. It has even more potential is we can find ways to use it or leverage it into some sort of method that enhances the product towards having the type of backwards (lets not say compatibility as that implies too much), call it capacity to open newer files, then that would save some users a certain amount of pain in the future.

Best regards

Hudson