Feature Parameters in NX9

[PSI-CAD]

I have found a problem with Feature Parameters during the Beta Test and I have opened a call.

Sample example: a sketch and an extrusion then drafting with master model

The following message appear if the sketch and the extrusion are not in the same layer and if the sketch is not visible:

Hidden features cannot be used for feature parameters in non-legacy views."


In the final release, the function is hidden by default and the problem is still there :

- Does it mean that Siemens wants to promote users to use the PMI Module ?
- But what about the users without this module ?


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

While it is true that the 'Feature Parameters' function is 'hidden' it has not been removed and can be easily activated using the Command Finder. And it appears to work just as well in NX 9.0 as it did in previous versions of NX. As for why it's 'hidden', I can't really say, but I'll try and get an answer for you from the people who are responsible, OK?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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[PSI-CAD]

Hi John,

The feature parameters doesn't work as it did in previous version of NX !!

Have a look at the given parts

Open sample_3D_NX8.5_dwg.prt (created in NX8.5) and try to use feature parameters ==> It works well (sample_3D_NX8.5.jpg)

Open sample_3D_NX9_dwg.prt (created in NX9) and try to use feature parameters ==> It doesn't work (sample_3D_NX9.jpg) Workaround : move sketch to layer 1 and unblank it

So, you confirm that the function doesn't work well with parts created in NX9 ?

Thanks in advance


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

I'm sorry Didier, but BOTH of your files work just fine using the production version of NX 9.0.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
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[Toost]

I (only) tried the NX9 version , in the production version , and i get the same results as Didier.

"Hidden features cannot be used for feature parameters in non-legacy views."

( If this is the difference.)

Regards,
Tomas

 

[JohnRBaker]

I get no messages whatsoeve. It just works. And I'm running the same version of the NX 9.0 that was copied to the GTAC download site. You need to contact GTAC and have them try it.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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Siemens PLM:
UG/NX Museum:

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

 

[JohnRBaker]

Are you using 'Partial Loading' or not? I was NOT using 'Partial Loading' but when I turn 'Partial Loading' ON then I can't access the Sketch feature in NEITHER the NX 8.5 nor the NX 9.0 version of the Drawing. Tha appears to be where the 'problem' lies, it's linked to the partial loading option. I recommend that you contact GTAC and have them open a PR.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[phillpd]

Testing in NX9, I see the same results as Didier and Tomas mention,

NX 6.0.5.3 (NX 8.5 Testing)
Windows 7 64

 

[JohnRBaker]

Have you read my last post concerning 'Partial Loading'?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[PSI-CAD]

Hi John,

If the partial loading is set, the features doesn't appear. So nobody are in this case to do the test at the end


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

I'm going to open a PR covering this issue. I'll let you know what I learn.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[peterrdevries]

Hello John,

Do you have the PR number, so i can attach mine to this one?

I really mis the Feature Parameters in NX9 for Sketches.

Thanks, Peter

 

[JohnRBaker]

I'm sorry, I never got around to opening the PR. I was on the road almost continuously during October and it just slipped my mind. SOrry. Please contact GTAC and have them verify the behavior that you're seeing and have them open the PR. Again, sorry.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[PSI-CAD]

Hi

Find herewith and attached the last answer (10 January 2014) of my call opened during the beta test (194812)

NX 9 introduced new functionality for creating Hole and Thread Callouts. This capability is supported for all view representations.*** 10-jan-2014 13:43:39 WINGRAVE, DAVID (wingrave) ***

Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

OK, I'm now running the production version of NX 9.0.1.3 (the MR which will be released in a few weeks) and I still see the issue with this behavior, depending on whether or NOT 'Partial Loading' is enabled in 'Assembly Load Options'. If 'Partial Loading' is toggled ON, then there is NO access to the Sketch when using the Feature Parameters Drafting function. However, if 'Partial Loading' is toggled OFF then I have NO problem whatsoever accessing the Sketch when using the Feature Parameter function.

That being said, I then decided to verify that this behavior had ACTUALLY changed in NX 9.0 and so I went back as far as I could, which at the moment is NX 5.0, tested this using a simple extruded part created from a sketch. And I discovered that NX 9.0 is behaving in EXACTLY the same manner as NX 5.0 (or for that matter, every version since at least NX 5.0), that is that IF 'Partial Loading' is toggled ON, you will NOT be able to access the Sketch using Feature Parameters. And it does NOT make any difference whether the Sketch is on the same layer as the extrude, whether the sketch has been made internal to the extrude and even if it had not and it was included in the Model Reference Set, it still will NOT be accessible by the Feature Parameters function IF the Master Model Drawing was opened with 'Partial Loading' toggled ON. This is just the way NX has ALWAYS worked (at least since NX 5.0). And when you realize what 'partial Loading' does, that is when toggled ON, Component feature parameters are NOT loaded when an Assembly is opened, you can understand why we're seeing what we are. The Feature Parameter Drafting function is, by definition, looking for the feature's 'parameters' but since they've not been loaded thry can't be accessed. Even if the Sketch itself is visible in a Drawing view, if 'Partial Loading' was toggled ON then the 'parameters' have not been loaded and therefore are not available to be inherited onto the Drawing.

So even if I did open a PR, it would come back "Working as intended."

Now as for the response that WAS given during the Beta testing, I suspect that the person who wrote that response did not fully understand what exactly was being asked. He was referring to the fact that annotating (i.e. dimensioning) Threaded Holes was now supported using a new explicit Hole Callout function which was added to NX 9.0 Drafting (as well as to PMI). However, even taking that into consideration, the response to the Beta testing PR was misleading since the Feature Parameter Drafting function STILL supports Holes, threaded or otherwise, just as it still does Sketch Parameters, AS LONG AS 'PARTITAL LOADING' IS TOGGLED OFF IN ASSEMBLY LOAD OTPTIONS. BTW, even the new NX 9.0 Hole Callout function is affected by the setting of the 'Partial Loading' option.

Anyway, I'm sorry that it has taken this long for me to come to the bottom of this issue since if I had followed-up when I first said that I would back in October, we all would have known what the status was then. As for the suggestion that this behavior was different in NX 8.5 verus NX 9.0, it would seem that if you went back and checked, I suspect that you will find that you were using NX 8.5 with 'Partial Loading' toggled OFF. And since out-of-the-box, NX 9.0 has 'Partial Loading' toggled ON, this is probably why you saw different behaviors between the two versions of NX. So, please check this out and let me know what you discover. Again, I'm sorry for not following-up when I first promised that I would.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cubalibre000]

John,
sorry, but what you wrote is wrong.
NX9 has a different behavior from the previous release.
Try to make a part and relative master model drawing in NX8 with partial loading enabled.
Import features parameters.
All feature can be imported.
Make the same in NX9 an all features aren't listed.

Thank you...

Using NX 8 and TC9.1

 

[uwam2ie]

Hey guys,
I missed a lot of the old unigraphics drafting shortcuts in nx9, I have called very early during the beta testing.Was closed it in septmember D.W. ,
Can't Duplicate, hope they get it fixed in NX901. The problem seems to be the time in software developement, testing. Give the Product managers a chance, in nx9 drafting/PMI is a evolution, many changes, maybe not ready in the final relase, thats the problem IMHO. BTW, found a workaround to switch arrangements in existing drawing views. I thought of a simple switch- we found greyed out in the previous releases. In nx9 style dialog there is nothing displaying what arrangement was used, hmm, enhancement or killed an idea to switch arrangements ... no way ;-) ...
you can inherit the arrangement form an other view with inherit view style in nx 9 ... not straight --- but it works ( for me).

 

[JohnRBaker]

I'm sorry, Cubalibre00, but I tested this in NX 5.0 up through NX 8.5 and it has always worked as I've described. Now don't be fooled by first opening the Part file, then creating/opening the Drawing and then adding the Feature Parameters since in that case the Part file is already fully loaded. Try starting a new NX session, set the Assembly Load Option to Partial Loading and THEN open the Drawing file itself. Now before you do anything else, try using the Feature Parameter function.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cubalibre000]

Jhon,
I'm sure that is change something in NX9.
Try to do these steps into NX8 (my company release at the moment):
1) Create a rectangle sketch with driven dimension (blu color)
2) Extrude the rectangle
3) Save
4) Create the master model drawing
5) Create a view that is parallel to the rectangle sketch, if not, feature parameter can't be imported
6) Import the feature parameter with the related command
7) Save and close

8) Open the drawing in NX9 and you can see that all dimensions imported with the feature parameter command are become 'retained dimensions'.

Now, our company use lightweight and partial loading setting in the load option, because the time to load assembly, in some cases is 70% better then standard options.

How can I switch to NX9 if all our drawings that have feature parameter imported, become disassociated ?

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

OK, I did what you suggested and got the same results that you did, however the problem is NOT with NX 9.0, as this same exact thing happens with NX 8.0 and NX 8.5. That is, if I create your suggested Model in NX 8.0 or NX 8.5 and then open the Drawing file in NX 8.0 or NX 8.5, with Partial Loading ON, the dimensions come in 'retained' just as they do if they're opened in NX 9.0 (or for that matter, if the part and drawing were created in NX 9.0).

Now I'm not saying that there isn't a problem, just that it apparently started in NX 8.0 since if you repeat this test in NX 5.0, NX 6.0 and NX 7.5, eveything works fine, even when I open those files in NX 9.0, the dimensions are there but NOT retained.

When I'm in the office on Monday I'll take it up with someone in the Drafting group and see what they have to say.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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