Customer Default Question 1

[DieMan44]

I'm trying to edit my customer defaults. One of the this I'm trying to do is change the way chamfers are called out by default. Currently, I get "C .25". I have to change it each time to ".25 X 45 CHAM". The default is set to size and angle, and the suffix is CHAM. But even after restarting UG, the customer default reads the setting I want, but I'm not getting that result. Help please!

 

[Xwheelguy]

Change your chamfer dimension Style default at the part level and save the part. Some customer defaults only affect NEW part files, not existing part files.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[ewh]

Where are the customer default settings for chamfers in NX5? I can't seem to find them (or section line defaults). The only settings I find have to do with colors.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[DieMan44]

So it's my templete file I take it. I need to change the settings in those file, save. Then when I use them, the defaults I want will exist?

 

[MCGNX]

DieMAn, I believe you can do either or. In fact there is a default setting that you can set to either take the defaults from the part or from the customer defaults file.

I believe the setting you are looking for though are in the customer defaults under the drafting standards, you can go into them and customize them all day long. You may want to save-as-new though so you can revert back if need be.

 

[Xwheelguy]

DieMan44,

You will have to open the seed/template file and change the chamfer style setting in Drafting and save the part file in order to change how Chamfer Dimensions are created. It might be wise to do a Save As and rename the seed part file to something different just to make sure it works OK for you, then replace the original seed file.

Like I said earlier, changing a Customer Default will mostly affect only NEW files, not files that already exist on disk. The files on disk are using whatever settings were used when that file was last saved.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[hudson888]

Somebody will confirm this for me because I'm commenting on something I think that I saw posted here previously, but haven't re-located.

The case in the past as I recall has always been that there are customer defaults which dictate the standards as applied to the creation on new parts, and then there are part defaults which lock on to settings that the part was created with, (i.e. other organizations have different site standards). So when you go into Annotation preferences and hit use defaults the settings are reset to the part defaults not your own local customer defaults. This is good for referencing the site standards from whence the part originated and is therefore a quite valid function. However many's the time when like most people I just can't live with the part defaults and have yearned to be able to hit a button which forced the part to swap over to my customer defaults. In the past I don't think this was provided for, but it may be implemented either in NX-5 or some upcoming versions?

Prior to that mostly we've created macros maybe journals or even Grip programs and the like to go through all the steps of forcibly changing a part to comply with our wishes in terms of how dimensions and annotations behave.

Maybe this goes to answer what Dieman44 really wanted to do.

Best Regards

Hudson

 

[JohnRBaker]

Yes that is true, some customer defaults control Session settings, which means that changing the default will effect all subsequent sessions of NX, while some are Part specific and therefore will only effect new parts created from scratch. We refer to this as the 'Scope' of the default.

Granted, there are some settings which are ostenisbly Part settings, but which there are options that will cause existing parts to be updated as well. I think you will find that many, if not most, of these defaults are in the Drafting area.

Now how do you find out which default item's Scope is a Session and which is the Part?

The easiest and quickest way to do that is to go to the Customer Default dialog and select the 'Find Default' option (the 'binoculars' icon near the upper right corner) and enter the term 'all' (without the quotes) and when the list is generated, scrowl to the far right-hand side of the listing and you will see a column titled 'Scope'. For each Default settable in NX, you find an entry indicating whether its Scope is 'Session' or 'Part'.

Now if you would like something a little more permanent to refer to, you could always export a copy of all the Customer Defaults settings to a spreadsheet, but be warned, this can take several minutes to complete. As of NX 5.0.3.2, there are a total of 9930 different Customer Default entries (and I won't even tell you how many there are in NX 6 except to say that it's a LARGER number).


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[DieMan44]

Hudson888, I like your sugestion. It's kind of related to my other post. Creating a journal (no grip compiling licence) linked to a button that would make the file defaults, mostly the drafting aspect of the file, to our standards. Have no clue yet on how to start that, but I think I'll work on that when I get the time. There are only two of us on NX3 and we really have no standards. I'm trying to correct that.

John, is it possible to link a journal to a spread sheet?

 

[JohnRBaker]

Yes, using Knowledge Fusion or if you're only reading values from the spreadsheet, you can use the Expression system and may not need to actually create any KF code, just the expressions and a Journal to apply them.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/