Surface finish symbols in NX7
Surface finish symbols in NX7
(OP)
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.
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.





RE: Surface finish symbols in NX7
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.
RE: Surface finish symbols in NX7
RE: Surface finish symbols in NX7
RE: Surface finish symbols in NX7
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.
RE: Surface finish symbols in NX7
Hope you fix this in the next MR....