NX8.5.2 Questions on new functionality & interface...

[Shadowspawn]

We just migrated to NX 8.5.2.3 and I have to admit to being very frustrated at the moment... I have a few questions regarding current and future functionality of the software that I can't seem to find an answer for and am hoping to find the answers here, so...
1) The new 'auto-translucency' behavior where the model goes translucent when applying features (blends, chams, etc...). I've queried ALL of our users and NOT A SINGLE ONE likes this behavior. How do I turn this off? Where is the setting?... I can't seem to locate it anywhere.
2) Sketches, specifically Geometric Constraints. ...Really? WTF happened here? The new interface is, IMHO and others, not intuitive and cumbersome to work with both initially when creating a sketch and while editing an existing sketch. This is a pretty big hit on productivity for our user base, enough to have been noticed by the pencil necks above/behind us.
3) Instance Geometry. It has recently come to my attention that this functionality is going away, and will be "replaced" with a pattern functionality of some flavor. I admit to not having looked much into yet, but our major concern is that our proprietary processes that gives us a competitive edge is very, very much based on the 'instance geometry' feature introduced in NX5.... specifically relating to the associative vector that the instance is based on. Change an expression controlling the vector, and the instance updates correctly. Prior to this functionality, once the vector was defined in the original pattern of the feature, it was forever written in stone and could not be replaced. Does anyone know, with certainty, that the replacement functionality for instance geometry will maintain the same functionality of the current instance geometry feature? This is critical!
4) Simple splines. The old fashioned ability to import a .dat file for spline generation, chaining existing points to generate a basic spline (that does NOT have to be associative), etc... I assume this functionality will still be available going forward, albeit buried someplace else. Can anyone confirm?
5) This is more of a general question... There seems to be a move by Siemens towards making everything associative, whether it's a simple line, bridge curve, basic spline, etc. Why is this? Is it not recognized that not everything NEEDS to be associative and so complex to create and edit? I get the idea and premise of 'increased functionality' and/or 'progress... moving forward' mantra that gets regurgitated.... but really, why can't the developers/TPTB understand that sometimes a line just needs to be a line and not all changes are a good idea, not all changes are wanted, nor are they necessarily a move in the right direction. /rant

I appreciate any answers and feedback to the above.... and as always, TIA

Regards,
SS

CAD should pay for itself, shouldn't it?

 

[Geardoman]

For your first question,

File -> Utilities -> Customer Defaults -> Gateway -> Visualization -> Emphasis -> uncheck the "See-Thru Preview"

 

[JohnRBaker]

OK, here's some feedback and answers:

1) You can disable the so-called 'auto-translucency' behavior by going to...

Customer Defaults -> Gateway -> Visualization -> Emphasis

...and toggling OFF the 'See-Thru Preview' option. However, I'm surprised with your comment that NOT A SINGLE ONE of your co-workers likes this behavior as that is the opposite from what I've generally heard form other users that I've spoken with on this topic, but then if we had felt all that hard-nosed about this, we would NOT have given you the option to turn it off, so in the end, it's your choice, not ours.

2) This has been discussed in detail in the past but I just can't put my finger on the response where I covered this. Basically the changes where made for two reasons, to leverage the new 'Shortcut Toolbars' which now provides immediate access to constraint options when you select sketch curves, and to provide an alternative workflow requested by legacy Ideas users who where used to preselecting which constraints that they wanted to apply before selecting the sketch curves. The only way to keep both the old UG/NX Object-Action approach and provide the new Action-Object approach preferred by the Ideas users was to completely rework how geometric constraints were applied, or at least the geastures used to initiate the various menu options. Again, once people learn what was done and actually start using it, it becomes pretty much a non-issue.

3) It is true that 'Instance Geometry' is being replaced by 'Pattern Geometry' in NX 9.0 based on the new 'Patterning Service' introduced in NX 8.0 with the new Pattern Feature function. But as for your concern, the new Pattern-based approach will still allow you to define the direction vector used in the 'Pattern' using the Expression-controlled vector option, no different than what you can now do with 'Instance Geometry'. The biggest reason for the NX 9.0 change was to make sure that all of the NX functions which creates multiple copies of something, which in the case of NX 9.0 will include, 'Pattern (Sketch) Curves', 'Pattern Features', 'Pattern Geometry', 'Pattern Faces' and 'Pattern Components', will now ALL be using a common interface, and in most cases, a common set of 'multiplicity' options. Once you get the hang of one of these functions, when you try another one, you will already be familiar with both the layout of the dialog and many of the options that are being presented.

4) While it is true that it will now take TWO steps to create a Spline from a text file containing X,Y,Z data points, it is in keeping with the idea that the new tools will be easier to use and much more useful in the long run. So the first step is create a set of points from your .dat file, This done by going to...

File -> Import -> Points from File...

...and selecting your .dat file. Note that this new function also supports several other common file formats used for imputing 3D Data.

Once this set of points have been created (which BTW will be a named group tagged with the name of the text file that the data was read from) you can then use it to create your spline by going to...

Insert -> Curve -> Fit Curve...

...and selecting the named group of points, the new spline will now be associatively linked to the points, meaning that if they are edited or if you replace one named group with another one, the spline will update. Also note that the new 'Fit Curve' function is not limited to creating only Splines, but will also allow the creation of a best-fit Circle, Ellipse or Line. And while we were are it, we also implemented a new ‘Fit Surface’ function which again leverages the idea of having functions using a common interface with common options, in this case allowing you to again select a named group of points, created using the Import -> Point from File function, to create a best-fit B-Surface, Sphere, Cylinder or Plane.

5) Yes, you noticed correctly. At least we don’t force you to create a sketch, like some systems are now doing , when all you want is a simple line or arc. Granted, the line or arc will be an NX feature, but at least they’re standalone objects which can be used just like their old non-featured curves of the past.

Anyway, I hope this helps you understand both the what and why some of these changes were made.


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.

 

[markrief]

What release did you migrate from?

Mark Rief
Product Manager
Siemens PLM

 

[Shadowspawn]

Mark,

Due to CAM needs (or so I'm told), we've gone NX6/7.5/8.0/8.5 within the last 18 months.


John,

Can we communicate offline regarding my concerns with the functionality we need on patterning/instance geometry? Or can you hook me up with someone I can speak to? I'm willing to provide complete examples and discuss/demonstrate what functionality we need via appshare. ...or whatever you think may help. So far, at least in 8.5, I'm not seeing a way out (we need to "pattern" curves/splines, not just features.



Regards,
SS

CAD should pay for itself, shouldn't it?

 

[JohnRBaker]

Have you tried calling GTAC?

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.