Standard selection filters is not that good when revolving or extruding.

[IvarA]

Hi

So i make this sketch and select the lines, I do use the select single line cause i only want to revolve certain parts of the sketch.
However the selection filter is set to none by standard. That means even the lines of the dimensional sign is possible to select, and that prevents me from selecting the line behind that I want to select. Who wants to revolve the dimensional sign anyway? Can I turn this off?

By dimensional sign I mean the thing that assigns the length or the angle in the sketch.

 

[JohnRBaker]

What version of NX are you running?

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, I think I see what you're seeing. Personally, I would just learn to ignore this since even if you did select a 'dimension' line it's not like it's going to be included as part of the profile when creating the Revolve feature. Just keep picking the stuff you want and all that other stuff will be ignored. Note that the reason we even allow you to select a dimension at that moment is so that if you suddenly noticed that a dimensional value was wrong or not what you now realize is incorrect, you could easily edit the value of the selected dimension WITHOUT having to leave the Revolve operation, enter the sketcher, edit the dimension, exit the sketcher and then start the Revolve operation over again. Look at how many steps and button clicks were just saved.

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.

 

[IvarA]

Thank you, but it is not possible to assign the dimensional sign or the line behind it. When i put the pointer to the line I want to sign, the dimensional line enlightens instead of the sketch one, however clicking on it does nothing..

 

[JohnRBaker]

Are you saying that the QuickPick menu is not working here?

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.

 

[SDETERS]

I have ran into this also. You need to watch what end and where your extension lines go when placing dimensional constraints. The reason I can see for this, is that you can select a dimension and change it while still in the Revolve command.

 

[JohnRBaker]

And you can use QuickPick to filter overlapping objects, just like nearly everywhere else in NX.

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.

 

[cowski]

A few ideas to resolve the problem:
[ul]
[li]use the quick pick list to specify the desired curve[/li]
[li]change your selection filter to "curve"[/li]
[/ul]

Or, my personal preference:
[ul]
[li]only sketch the geometry that you want to revolve or extrude, then use the "feature curve" selection rule[/li]
[/ul]

If you have any construction geometry in the sketch, specify it as "reference". Any reference geometry in the sketch will be ignored for operations such as revolve, extrude, sweep, etc. When you later edit the sketch and add new geometry, it will automatically be picked up by the "feature curve" rule; no need to edit the extrude to select the new curves that were added. Other sketches can reference geometry in this sketch if needed.

www.nxjournaling.com

 

[Xwheelguy]

A few ideas to resolve the problem:
[ul]
[li]use the quick pick list to specify the desired curve[/li]
[li]change your selection filter to "curve"[/li]
[/ul]
Or, my personal preference:
[ul]
[li]only sketch the geometry that you want to revolve or extrude, then use the "feature curve" selection rule[/li]
[/ul]
If you have any construction geometry in the sketch, specify it as "reference". Any reference geometry in the sketch will be ignored for operations such as revolve, extrude, sweep, etc. When you later edit the sketch and add new geometry, it will automatically be picked up by the "feature curve" rule; no need to edit the extrude to select the new curves that were added. Other sketches can reference geometry in this sketch if needed.

^^^^^ X2.​

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[IvarA]

Yes i use the quick pick or just change the selection filter. But having to do that all the time is tiresome. I prefer making extensive sketches.

 

[Toost]

What happens if you press "Ctrl+Q" ( = Finish Sketch) before you start the "Revolve" command ?

 

[GaryFisken]

A few ideas to resolve the problem:
use the quick pick list to specify the desired curve
change your selection filter to "curve"
Or, my personal preference:
only sketch the geometry that you want to revolve or extrude, then use the "feature curve" selection rule
If you have any construction geometry in the sketch, specify it as "reference". Any reference geometry in the sketch will be ignored for operations such as revolve, extrude, sweep, etc. When you later edit the sketch and add new geometry, it will automatically be picked up by the "feature curve" rule; no need to edit the extrude to select the new curves that were added. Other sketches can reference geometry in this sketch if needed.

This is yet another stupid design decision from the NX development.

The only real solution is to change your selection filter to "curve" since it's often useful to make several features out of a single sketch.

Is it possible to change the default setting for this?

 

[IvarA]

@JohnRBaker im using NX 9.5
@Toost yse I do exit the sketch.


I know that there are workarounds for the problem I have, such as selecting "curve" in the selection filter. But in 96 percent of the cases that is what you want to while revolving etc. So why not set that as a standard anyway? Problem right now is that I have to select the "curve" filter every time I want to feature.

 

[Crocostimpy]

@GaryFisken

Yes you can change the default behavior. Go into your Customer Defaults. Go to Modeling - Selection Intent Rules. Here you can select what the default behavior will be when you start a creation command. Revolve is under Design Feature. Select what you want it to be from the dropdown menu.

Mike