simple section thro holes 2

[GPowers2]

people,

NX4 user - I have two holes running parallel and wish to take a section thro the centres, I select section view .. pick the view (up come the arrows etc) .. I then pick the ctr of one bore ... then I am unable to pick the centre of the second bore.

this has got to be easy but I cannot find the answer ..

regard ... gary

 

[jackley]

Don't you have a animated section line when you move the mouse around after picking the center line of the circle? It should also snap when the view is projected vertically or horizontally.

I'm still in NX3.0 and I can't imagine it's changed.

Justin Ackley
Designer

 

[ewh]

Accept the section line through the first hole and place the section view. Edit the section line to add a segment through the second hole.

 

[GPowers2]

I do get the animated line that spins around the initial 'centre of bore' pick, by NX4 does not allow me then to pick the 'centre' of the second bore thus insuring a section thro the two bores ....
(NB: they are not perfectly horizontal or vertically aligned )..

 

[GPowers2]

editing the section line and adding a segment will not allow the accurate distance between the two bores to be dimensioned ... which is ultimately what I need ........

 

[JohnRBaker]

OK, here is how you do this.

Select the view you wish to define the section in and hit MB3 and select 'Add Section view...'.

Now you will see a preview of the section line that moves with the cursor and the prompt is asking you to 'Define cut position - Specify inferred point'. Select the center of one of the holes.

Now select the 'Hinge Line' option on the Dialog Bar. When you do, the option next to it, 'Inferred Vector', will become active (no longer grayed-out). Select it and from the list of vector methods, select 'Two Points'.

Now select the center of the first hole feature and then the center of the second hole feature. Now you will see the preview of the section line pass through the centers of the two holes.

At this point the direction of the section arrows may not be correct for the location where you wish to place the section view, so if it's wrong, just select the 'Reverse Direction' option on the Dialog Bar and then place your section view, which will now show the true distance between the two holes.


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/

 

[GPowers2]

Mr John R Baker that was a great answer and worked fine...

appreciate the help ....

regards .... Gary