Changing Part units in NX5

[Joshmo]

Hello all,

I am a new NX5 user and ran into a problem I would think would be simple to figure out but got a little stumped. I made a part in mm but later wanted to swith it and all the dimensions to inches. The only way I found to do this was by using the NX command prompt and typing: eg_convert_part _inch partname.prt

I then think I had to scale all the part dimensions manually which was a pain in the ass. Is there an easier way to do this other than going to the command prompt? If not they need to make it easier in future versions because even low level programs like autocad can change part units easily.

 

[JohnRBaker]

Based on a very old standard that even today makes itself known in products like IGES and STEP tranalators, NX part files are stored with either Inch or Millimeters as the 'base' unit. And this can NOT be changed except through the use of the external utility, 'ug_convert_part'. Besides resetting the base units, this utility will also scale all geometric objects so that their absolute size is maintained. That means that if I had created an Inch part and created block 4 inches on each side and I then ran this part file through the conversion utility, I would now have a Millimeter part file with a block that was 101.6 mm's on each side.

However, starting with NX 3, the expressions used to define the original block would still read 4 inches, since starting in NX 3 expression values included both units and dimensionality, and since the actual units specified in an expression is now considered as the user's 'design intent', we no longer modify the original parametric specification. However, any subsequent contruction will now be done in Millimeters, unless you have set a local (and temporary) construction unit, found under Analysis -> Units..., to something other than Millimeters. Note that these construction units have no effect on the actual 'base' unit of the part file, but merely defines how parameters are to be interpreted and stored (as expressions) as well as reported when a model in analized or measurements are made. These settings only remain valid for the session and the part will revert to where the construction units match the 'base' units the next time that file is opened.



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

http://www.siemens.com/plm

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