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NX Routing Mechanical, Make Holes on Steelwork Stocks




I need to make some holes Normal to one of the four faces other than the two cap faces of a Hollow Square Beam created with Routing Mechanical and using the Steelwork Stocks. Issue is that when using the Modeling-Hole tool, and the tool asks to first click on the surface where the hole would be, NX doesn't recognize the faces of the HSS neither as a Face, Facet Body nor Solid Body, so those faces are unselectable and only recognizes as selectable the cap faces. On the part navigator this beam appears only as Stock (XX), so can't tell if its a Solid Body or Sheet Body or Facet Body. Your help would be much appreciated. Thanks!


Re: NX Routing Mechanical, Make Holes on Steelwork Stocks

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor



It almost sounds as though the face of your square stock is not planar.  Select "Menu > Information > Object", change your Selection Filter to "Face" and then pick the face that your trying to add holes to and then hit OK on the dialog.  The Information window will report something similar to:

Type                 Face
Color [from body]    129 (Medium Steel)
Font                 SOLID
Width                0.70 mm
Modified Version     3     07 Dec 2017 08:50 (by user broad)
Created Version      3     07 Dec 2017 08:50 (by user broad)
Information Units    mm
Surface Type         Trimmed Planar

What does it report for "Surface Type"?

Regards, Ben


Re: NX Routing Mechanical, Make Holes on Steelwork Stocks

Siemens Genius Siemens Genius
Siemens Genius

Hello Maruz,

It's a solid body.  Routing only creates solid bodies.  The Part Navigator in Timestamp Order mode only shows features.  Like an Extrude will show as an Extrude feature regardless of whether it's a sheet or solid result.   Turn off Timestamp order mode, and bodies will be listed and then expand to the parent features.


But on to your issue.  There are two modes for stock bodies made available by the root parasolid feature.

The default takes all tangent curves in the cross section and makes a single b-surf when it sweeps the solid.  Nice looking and accurate, but doesn't act like the planar and blend surfaces I think you are expecting. 


In Customer Defaults, Routing, General, Stock tab, change to Create Tiled Faces for Stock Bodies.  This will give you a face for each curve in the cross section.    Once you change the setting and relaunch NX, any updates to stocks will give the new setting.


There is a drawback to it though.  It also creates face along the sweep at each path segment.  So if you subdivide a linear segment, you'll see edges there, too.   We have just recently determined that there's another method available to us that will merge the faces along those collinear path segments.  We'll introduce that in an upcoming MR/MP.  Later we'll clean up the current CD settings and default mode.