Continuous auto dimensioning 2

[Karlis]

Hey everyone,
I have two simple questions regarding this topic in NX9.0

1) How can one save the settings in sketch preferences so that every time I open NX I get the desired settings? To me it always resets to defaults.
2) How can I remove the fake dimensions from my sketch once I have turned off the auto dimensioning? To me it keeps creating the fakes even after I have dis-checked the "continous auto dimensioning" in sketch preferences.

I would really like to solve these issues because my sketches are complex and handling them really eats some CPU resource.°
Thank you very much

 

[JohnRBaker]

To disable 'Continuous Auto Dimensioning' go to...

Customer Defaults -> Sketch -> Inferred Constraints and Dimensions -> Dimensions

...and at the bottom of the page you'll find the options to control the behavior of 'Auto Dimensioning'. Note that these are SESSION specific settings which means that once they are toggled ON/OFF, this option will be toggled ON/OFF for BOTH new files being created and when opening an existing part file, even if is was was created prior to when we introduced this capability in NX. Remember as always, once you make any change to Customer Defaults, you have to save the changes, exit your session and restart NX for these changes to take effect.

As for removing the so-called "fake" dimensions (BTW, they are NOT "fake" as they are really helping to constrain the sketch, just that they are NOT 'driving' dimensions) you have only two choices, either explictly delete them (and once the Auto Dimensioning option is toggled OFF they will not reappear) or double-click them and they will be converted into normal sketch ('driving') dimensions.

Note that this last item, editing an Auto Dimension to convert it into a Driving dimension, beings up a powerful way to use this capability. Once you've set the Auto Dimension option to be OFF by default and while you're creating your sketches, you mention that your sketches are very complex, I'll bet that there are times when you're adding constraints and dimensions to a sketch and you just can't seem to find those last two or three dimensions that will fully constrain your sketch and you wished that the system could provide you with just a bit more feedback as to what you should try next. Well this is the prefect time to go and toggled ON the Auto Dimension option and see where the SYSTEM adds any new "fake" dimensions, as you call them. These dimensions, if they were actual 'driving' dimensions, would have fully constrained the sketch. You can either accept them by editing them into 'driving' dimensions. or at least use them as a hint as to where you might need to look to find what part of the sketch needs some additional constraints and/or dimensions. This is how I, and many other more experienced users, have come to leverage the Auto Dimensioning function, using it as more of a 'tool' that can help us clean-up those last few bits that needs to be done before we have a fully constrained sketch.

Anyway, I hope this helps.

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.

 

[Karlis]

Hi John,
It is actually strange, but once I toggled the continuous auto dimensioning offlike you instructed, they just keep reappearing again and again. I tried converting them into driving dimensions and then deleting them, they still reappear even after I restarted NX.
I have also noticed that sometimes after deletion, they appear in double, and I cant get rid of them. I really do not want to redraw my sketches..
This only happens to he sketches that have been created with the "continuous auto dimensioning" option on, which was toggled off after their creation.

 

[cowski]

After you make a change in the customer defaults, you will need to close and restart NX for the change to take effect.

www.nxjournaling.com

 

[Karlis]

Hey cowski, I did and it did not help. I already mentioned that.

 

[cowski]

In addition to the customer default setting try changing:

Menu -> preferences -> sketch -> sketch settings -> continuous auto dimensioning - toggle this setting off (if it isnt' already). This should change the preference for new sketches.

And...
Right click the sketch, choose "settings" and turn off the option there. This should disable it for that particular sketch.

www.nxjournaling.com

 

[JohnRBaker]

If you make the change I mentioned in Customer Defaults, this is a 'SESSION' specific setting which means that it will affect all future sessions of NX, even if the part file already exists. Also make sure that changes that you're making to Customer Defaults is at the 'User' level since if it's being done at either the 'Site' or 'Group' level, the settings in the 'User' level Defaults will take precedence.

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]

It is a session setting, but it also appears that it is saved "per sketch". Changing the preference does not seem to affect sketches created before the change as you would expect a "session" setting to do.

Exit out of the sketch task, right click -> settings, and turn off the option there. Now when you edit the sketch, the previously added "auto dimensions" still show up but they can be deleted and no new "auto dimensions" will be created as you edit the sketch.

www.nxjournaling.com