Preference for individual centerline extensions 1

[MEichWey]

Hi,

I´m searching for a preference to set the centerline-extensions to individual extensions, so that I have on each centerline-point 4 extensions to all directions. In the dialog under settings I can switch it on and off. But I didn´t find any preference for it. Not in the customer-defaults and also not stored in the part, e.g. in the seedpart. Do anyone know a solution? Maybe is there an OS-setting like "UGII_CENTERLINE_EXTENSIONS_INDIVIDUAL" = ON or OFF?

Regards
Michael

 

[SvenBom]

I don't know if there is a setting for this. But you can save your own dialog box settings.
1. click on Center Mark command
2. select 'set extension individually' option
3. select and set any other option, that you need
4. click on 'Dialog options' on the top-left corner of the dialog box.
5. select 'Save Favorite As'
Now, when you select Center Mark next time, you can click on this Dialog options and select your saved favorties. Or, you can go in tools/customize and place your saved favorite as new command in your toolbar. Then, you are using this new command instead of Center Mark.

 

[MEichWey]

Hi Sven,

I found a preference in the customer defaults - under Drafting -> Annotation -> Symbols -> Centerlines. There I can setup the "Show All Extension Handles" to On and Off. But it doesn´t work (NX8)! The solution with the favorite is a workaround, but not very good. With changing to the next Version of NX we have to do the same. So every time it is better to have a fix setting for all users and not to change something in existing Toolbars. Favorites are normally for Workflows where users multiple times have to create Features with same values but not to set preferences.
I would like that Siemens will put any preferences in the customer default with a choice of system-setting or part-setting.

Best regards

Michael

 

[MEichWey]

Hi Sven,

how is it possible to set a favorite as a new command into a toolbar?

Michael

 

[SvenBom]

I have checked the customer defaults as you suggested. I did this in NX8.5 since I don't have NX8. And this setting is working.
1. customer defaults as you suggested. I have turnde on 'Show all extension handles'.
2. restart NX
3. open new drawing
4. draw a circle or create a view from a model.
5. select the Center Mark command. In the center mark dialog box, under settings, the option 'Set Extension Individually' is not selected.
6. place the center mark on the circle.
7. all four arrows on the center mark are visible.
And this is exactly what this customer default settings ('Show all extension handles') is doing. It is just showing all four handles.
Unfortunatelly, I still can not find any setting for 'Set Extension Individually'. And I agree, it would be nice to have this option, too.

 

[MEichWey]

Hi Sven,

thank you! Now it works - also in NX8. As I set the preference in the customer-default, then restart NX and open the dialog with the setting which is off, I thought, that it doesn´t work. But it is crazy that it does the opposite as the dialog told me.

Thanks

Michael

 

[SvenBom]

Yes, but even though you can see all four handles, you can not extend them individually. It doesn't matter which handle you move, all four will move the same.
Customer default setting is 'Show all extension handles'. And this is exactly what it does. It just shows all four handles.
But the dialog box setting is 'Set Extension Individually'. With this setting, you can move all extension differently.
Did you just want to see all four handles?

 

[SvenBom]

Only now I have seen, that you have also asked how to set the favorite as new command.
I have uploaded a movie, where you can see, how this is done.

 

[MEichWey]

Hi Sven,

that´s very good. I didn´t know before how to do that.

Thanks

Michael

 

[JohnRBaker]

No there is NO option, Customer Default or otherwise, which will force the 'Set Extension Individually' option to be toggled ON by default. The Customer Default setting to 'Show All Extension Handles' was provided only because some people felt that highlighting a single handle might mislead people into thinking that ONLY that extension line was going to be changed. It was felt that the if we showed all four handles that it would be less confusing and besides, users could then select whichever handle was most convenient for them. Of course, some of us felt that we should ONLY show all four handles when the user is actually able to edit WHICHEVER extension that they wished to, hence the reason why the 'Show All Extension Handles' option is OFF by default.

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.

 

[MEichWey]

Hi John,

why it is not possible to put all preference setting to one location. We have settings in the Customer Default, in the Part, in Users OS-Profile and Windows-Registry. But not all of them can bet set as a preference. This is very confuse for all User and me too, cause no one knows where a preference has to be setup. There is no documentation, which setting can be set at what location. As I testing NX10beta, I see that it is the same in that version. I thought, that it will be much easyer to have them only in customer default and also to have the ability to set them all. Some dialogs are also from "older" versions and have no "Favorite"-options.
Will it be a way to do that in one of the next versions of NX?
The best way would be:
All settings in customer default and additional at each setting a checkmark for "in Part", "General" and "User".

Michael

 

[JohnRBaker]

This, like a lot of things dealing with what are known as 'Gateway' issues, things which are UI in nature or which provides common functionality and behavior, like selection, display, preferences, etc. are a 'work in progress' meaning that we work on it continuously with projects funded for each release but there is no one single big project to change everything at once. For example, in NX 9.0 we introduced the new Ribbon interface, but there are projects in NX 10.0 to fine tune some of the features associated with new interface and we expect that there will be some additional work in NX 11.0 as well. Also in NX 9.0 we completely revamped all of the Drafting Preferences combining several different dialogs into a single new 'settings' format which will be the model for when we update the preferences dialogs for other areas of NX as we go forward. For example, in NX 10.0, the User Interface Preferences got this new overhaul. We're also working on making the Customer Defaults presentation more consistent with what you're now starting to see with the changes that we're making with preferences.

As for some of your other issue, there will always be a separate Customer Default and Preferences set-up. Customer Defaults are intended to be just that, the place where you set what the CUSTOMER wants to see as THEIR 'Defaults' when he starts a new project on NX. Preferences are for things which fall into one of two categories; items that one might wish to change while in the middle of a project or even while working on a specific part file, such as Display setting, selection options, tolerances, etc. And then there are the items which will be saved with the Part File itself which while Customer Defaults might have covered 90% of the cases, there still might be some specific changes that one might want to make which is then saved with that part file but which would have no effect on any other part file already created or which might be created in the near future.

As for the use of the 'registry', again there are certain things that just makes sense such as anything which might be relevant to the particular workstation that you're running NX on, it only makes sense that these setting should stay with the workstation even if their initial 'out-of-the-box' settings were first determined by Customer Defaults. And even here we are constantly changing, reducing what we are using the registry for. Years ago, much more was being saved in the registry than today. Again, another example, in NX 10.0 we've implemented new options to control the content and appearance of the Resource Bar and its 'tabs'. In the past any changes to the Resource Bar were saved in the Registry, however, starting with NX 10.0 these will now be saved in the .mtx file like most other settings and UI preferences, which means a couple of things. First off, since the .mtx file can sort things by application/task, the Resource Bar settings can now be set to specific options on a per Application/Task basis. Also, since these are now saved in the .mtx, that also means that you can have different Resource Bar settings in difference Roles, which also means that it will be easier to save them for use by other people in your organization.

So you see, we are making progress, slow though it may seem as it's an ongoing effort, but it's one with a limited amount of funding and even that funding most be weighed against how we're funding all of the other projects which make-up the effort put forth for each new version of NX.

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.