NX9 Highlight/Selection order 1

[johnwizz]

Hi Everyone!

I believe this is the first time I have posted in this forum, although it has been extremely helpful finding answers!!! Thanks to all those who have contributed!!!

Our company just switched from NX 7.5 to NX 9 and as you might imagine we are having a lot of fun working through the transition! Ugh!

One of the items we have run across is this...

When you pass your mouse over an item and select it, NX7.5 used to select the last operation that was done to that item. So for example, if I selected a studio surface that I had extended and then trimmed, NX7.5 would have picked the trim function which I could then delete or edit. Now if I do the same thing NX9 selects the original studio surface or I have to choose to select from a list and try and find the operation I am looking for. In a smaller model this isn't that big of a deal, but in very large models which we work with regularly it is very time consuming and aggravating to say the least.

I have tried multiple searches both from google and on this forum and haven't been able to find anything.

If anyone can tell me how to get back to the way it used to be, I would be very grateful!

Thank you,
John

 

[cowski]

Check your "selection priority" setting in NX 7.5 vs 9 to see if they differ.

www.nxjournaling.com

 

[johnwizz]

Hi cowski, Thanks for responding!

That doesn't seem to make a difference. Even if I set it to "Feature" it still selects the "parent".

 

[MickyV007]

RM button on the part navigator name column then properties. In the general tab of the part navigator properties menu, there should be a setting 'Automatically scroll to selection', should be checked. I don't know for NX9 but the setting is in 7.5 aswell in 8.5.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[johnwizz]

Michael, thank you for the reply. That is checked already.

I'm not sure if I am explaining my issue correctly or not. Let me see if I can clearify...

If I have a surface (the "parent") and have modified the surface with several operations (like trim and/or extend)(the children). While in the main modeling window if I pick the surface (LMB), NX7.5 would select the last child while NX9 selects the partent. I'm trying to figure out if there is a user setting to change this.

Sorry if I am being unclear. I am not sure how else to explain it.

Thanks agian!

 

[cowski]

Does this happen with all features or just trim/extend?

I ask because there is an option within trim/extend called "extend as new face". If this is turned on and you select the new face, the trim/extend feature will be selected; if it is turned off, there is no new face and you can only select the parent feature (unless you use the quick pick dialog). Perhaps this option was turned on in your install of 7.5 and it is turned off in 9?

www.nxjournaling.com

 

[johnwizz]

No it's anything. Seems like NX9 defaults to selecting the parent no matter what has been done. I don't think I have found any instance where NX9 does not select the partent with out using the quick pick dialog (which can be a pain).

Another example would be a curve extruded into a surface that has been trimmed to another surface using the Trim Sheet command. NX9 will select the extrude vs the trim. NX7.5 would have selected the trim.

Thanks!

 

[Arkance/PhoeNX]

I can't replicate the behaviour in NX7.5 that you said you had.
NX7.5 and NX9 are the same for me and I ran the OOTB defaults.

See the attached video that shows they are the same.

If NX7.5 is different, then you've changed a setting so I would try an get access to the old customer defaults you set and see if there's something you have set.


Anthony Galante
Senior Support Engineer


NX3 to NX9 with almost every MR (18versions) plus the NX10 Beta

 

[johnwizz]

PhoeNX, thanks for your answer. I see what your showing but that is not how my NX7.5 used to act. Unfortunately I have no way to see the old defaults. I was hoping that someone on the forum would have already run across this and would be able to tell me what setting this would be.

Thanks agian!

 

[opetrenko1]

this thread in top google results
has been solution to this problem found?
this new feature (or bug) is quite irritating
Thanks!

 

[JohnRBaker]

Technically, t's only a 'bug' if it can be reproduced. If there's only person experiencing this issue and others say that they see NO difference between NX 9.0 and older versions of NX, then it has to be something that is set differently in your copies of NX. Until it can shown that NX 9.0 or NX 10.0 actually works differently than XN 7.5, there is nothing that can be done. I would recommend that you contact GTAC but again, if you can't demonstrate that there has been a change in behavior there is very little that we can do.

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

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

 

[opetrenko1]

Thank you, John.
I agree with you and confirm that NX8.5 is just as well select the very first ancestor rather then the youngest kid.
I switch from NX6. ( And NX4 before it. )
NX6 selects the latest of the kids and it worked very well for me as it's the last features that usually get modified. Contrary, selecting very first ancestor body has no value at all, as list of its dependencies contain features of from other bodies as well.
am I doing something wrong? Do I have to select from the list everytime I need to modify current feature?
Thanks

 

[JohnRBaker]

OK, I've gone back to NX 5.0 and discovered that in the case of Sheet bodies, where additional featurea have been added to the body, such as an X-Form or Enlarge feature, that when you then attempt to select a feature, the most recent, and NOT the base sheet body, is selected first. And while it was a bit harder to come-up with a similar scenario for features being added to the face of a Solid body, I did try both Offset Face and X-Form (at least starting with NX 7.5) and they behaved the same, at lesat until NX 7.5 when for Sheet bodies the order did indeed reverse while for Solid bodies it did not, it remained the most recent being selected first. What I think is happening is that in the case of the Solid body anything you do to a face of the body actually creates NEW 'geometry' and so that will Always be seen first, while with Sheet bodies, there is NO new geometry simpley the old geometry is changed so it now depends on what the software sees first. That being said, it appears that starting with NX 7.5 someone changed the selection behavior to say that if there is NO new geometry, that NX will place the priority on the feature where the actuall body residesm, which if whatever feature created the original sheet body, in my test case that was a Swoop surface.

Note that I checked all versions of NX from NX 5.0 thru NX 10.0 and it appears that this change in behavior, at least with respect to Sheet bodies, occurred with NX 7.5. I talked to the developer responsible for selection and he's not aware of any changes being made except that it's possible that someone 'fixed' something somewhere else that changed this behavior since in reality all that selection does is take the feature that is highlighted so it could be that code that's impacting the selection priority.

Anyway, my advise is that if anyone feels that this priority is wrong then contact GTAC and have them open an IR/PR since you can site both the idea that this is a regression as well as inconsistent with respect to how the highlighting works when an X-Form feature is added to a solid face. The behavior is inconsistent in that, at least starting wth NX 7.5, the priority of selecting an X-Form feature added to a Sheet body is different then it is if applied to the face of a Solid body.

So while I'm not really ready to call it a 'bug', since one could make the case for either behavior, since it does seem to be something that has changed and since it appears to behave differently whether the extra features were applied to a Sheet body versus a Solid body, that would support the argument that we need to change this back to the pre-NX 7.5 behavior.

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

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

 

[JohnRBaker]

OK, we uncovered what happened. Back a few years ago apparently someone opened a PR because they thought that the order of selection in NX 6.0 was wrong and that the base Sheet body should always have the top priority, so they changed the selection behavior. However, there was some debate as to whether this was such a good idea so they gave themselves a back-door. Now it seems that very people ever noticed this change so nothing more was done except to have an environment variable to set it back to the old behavior, so if someone complained about this, we simply offered them the variable, and while I'm not a big fan of giving these 'variables' out willy-nilly, I'm going to just that in this case. So if you set the following variable to ANY value, you will get the old behavior that when selecting features imposed on a sheet body, that they will be selected in the reverse order of when they were applied (i.e., latest first), which is what happened prior to NX 7.5:

UGII_SELECT_LATEST_SHEET_FEATURE=1

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

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

 

[opetrenko1]

That's quite an invetigtion!
Thank you, John!