Unite fails because thru face does not intersect path of the tool

[godpaul]

nx 8.5

i tried to unite a cylinder and a swept geomeetry (picture1), but failed.

i kind of know the reason because one dimension in the sketch for the swept is set as EXACTLY equal to "diameter/2". I assume the unite operation would be successfull because the sketch is perfectly attached to the cylinder based on the dimension i specify. the reason i do this is i use the same modeling method in Inventor and no trouble for me...

Now, in the NX, it's a fail operation.

one way to avoid this issue is to make the dimension of the sketch just inside the cylinder, say "diameter/2 - 0.1" so that later on swept operation intersects with the cylinder and then i can unite. but i dont like this way....


Is there any better way to avoid this issue?

thanks



pic1

http://files.engineering.com/getfil...-3ad2-422c-9d68-a9e50a206dcf&file=Capture.PNG

pic2

http://files.engineering.com/getfile.aspx?folder=59975560-8f04-4f4c-8a96-e0bce5a29017&file=2.PNG

model

http://files.engineering.com/getfil...2-9635-dfd89e7e9e54&file=testDrawingModel.prt

 

[JohnRBaker]

While I did get the same message that you did when attempting a Unite operation using NX 8.5.3.3, when I tried the same thing using NX 9.0, it worked just fine.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[godpaul]

NX 8.5 bug?

 

[wacio]

Hi. I have suggestion. I cant open your part - using 7.5, but you could try to replace face that sits against cylinder (probable bsurface) with the face of cylinder and than try to unite again.

NX7.5 + TC8.3

 

[Toost]

Obviously new algorithms in NX9. Brilliant !

The 8.5 behaviour is not a bug but how NX works in older versions.
You are trying to unite a highly complex Nurbs face , which is using a tolerance, to an exact cylindrical face. The Nurbs face is not identical to the cylinder, it has small undulations within the tolerance which might be both inside the cylinder as well as outside. In older versions of NX these faces must be either identical or overlapping, else the Unite operation fails.

The comparison to Inventor is completely irrelevant. Inventor uses a different modeling engine than NX. How a specific feature is implemented in the cad system can be / is completely different as well as the algorithms in the modeling engine itself. Parasolid can do some things which Inventor cannot and vice versa.


Regards,
Tomas

 

[godpaul]

Thanks for all of your comments and i should be careful when performing this feature in 8.5, hope we will upgrade to 9.0 soon.