Surface finish symbols in NX7

[eex23]

Hello,

There is smth wrong with surface finish symbols in NX7 (i believe also in NX7.5). If you will look to the attached pdf file, you will see, that marks (a,b,c,d,e) are in different places than NX offers, according to the DIN EN ISO 1302.
Is it going to be changed?

Thanks.

 

[uwam2ie]

It's not the same surface finish symbol in nx7 or Nx7.5.
You can configure these places in nx7 use the drop down, maybe you have to change the base setting roughness grade to micrometer - than you find what you want.

 

[eex23]

The problem is not micometers. If you wil study ISO 1302 standard, you should pay attention, that places for the marks a,b,c,d,e are different, eg a1 and a2 in NX are not allowed in ISO standard at all.

 

[uwam2ie]

a1 ,a2 are only placeholders leave them blank in the dropdown for a1, a2... only options to use what maybe not covered in the iso 1302 standard . Use only b, c/f1, e , d , f2 and you get what you want. Ok it is not the same lettering as in the standard - thistransformationshouldbenoproblemforyou

 

[JohnRBaker]

To start with, unless you're working with NX 7.5.x.x, you don't really have any usable Finish Symbol functionality. So let's first assume that you're using something like NX 7.5.2.x.

OK, so what you need to do is to go into...

File -> Utilities -> Customer Defaults -> Drafting -> General -> Standard

...and then select the 'DIN(Shipped)' Drafting Standard and then push the 'Customize Standard' button. Now go to...

Drafting Standard -> Surface Finish Symbols -> General

...and change the standard from DIN 1992 to DIN 2002. Now you will have to do a 'Save As' from this page and give a new name to the DIN standard file, which will become the new default once you leave Customer defaults by hitting OK and restarting NX. Note that there is no way to edit the as-shipped version of the DIN standards file from the interactive dialogs.

Now if you prefer, I've attached a new updated copy of the 'as-shipped' version of the NX 7.5 DIN drafting standard file (nx75_DIN_Drafting_Standard_Shipped.dpv) already modified so that the 2002 standard is preset. If you would like, just download this file and go to...

xxx/UGII/drafting_standards

...and replace the file with the same name that you find there. Now you will still need to go back to an NX 7.5 session and make sure that in Customer Defaults that the 'DIN(Shipped)' has been set as the default standard and that NX has been restarted. If you either the interactive edit procedure outlined first above or go the replace the current as-shipped file route, when you now go into the Finish Symbol dialog this is what you should see...

...which I think you will see is consistent with your standards document.

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

http://www.siemens.com/plm

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

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

 

[uwam2ie]

@John take a look at the nx6 release,first you have to activate the surface finish symbol in the ug_env.dat.an issue in 7.5: The (legacy) surface finish symbol is flipping text when it is rotated to 180° - the 7.5.2 doesn't. But fipping the text is industry standard - also if it placed on the dimension extension lines it isn't fixed to the dimension extension line (it should be, the legacy symbol does).
Hope you fix this in the next MR....