Section Hinge Line orientation

[Spankpapa]

Hi, some help would be greatly appreciated !

I'm inserting a secion view in a drawing.
I pick the parent view, then I want the hinge line to be perpendicular to a curve in the view. Whichever way I try to do it, I only seem to be able to set the hinge line to follow the curve.

I know it's probably basics, but it's pretty frustrating !

I've tried messing with IJK values, and also with Theta vaules in one of the associated vector construction menus, but I'm having no joy !

Any ideas

Thanks

Papa

 

[morans]

I don't know how or why UG picks the direction that it does, but I often have problems with this myself. Usually if it wont pick the direction properly I'll use the 2 point method instead (or draw a curve in, 90* to the original). It's probably not the best way to do it, but it's never been an issue in the years I've been using UG.

hope this helps.

 

[HGE]

Spanky,
Use the "Oriented Section View" function to create your section view. I think this will give you what you're looking for.

 

[JohnRBaker]

At least with NX 5.0 and NX 6.0, after selecting the Parent View, and the your dialog options come up, in the section titled 'Hinge Line' rather then use the default 'Infer Hinge Line' option select the 'Define Hinge Line' icon and from the list of 'Inferred Vectors' select the 'Face Normal' option and then you can select any planar 'face', which could be represented by that 'line' you want to section normal to (you may need to use QuickPick to get the actual 'face' that you wish), or the 'face' of the cylinder or cone to section normal to. Anyway, if you really have some 'feature' of the model which you wish the orientation of the section to be relative to, you really need to check out the flexibility available to you using the the 'Defined' as opposed to the 'Inferred' method of selecting a reference object.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
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.

 

[Spankpapa]

Hi,

So, further to yesterdays' cry for help, I'm on NX4, and it's actually a curve/basic line that I'm wanting to use to orient the section hinge line. It's a line from a sketch that I'm selecting.

Morans, yeah I'm not new to Ug, and I've been using the 'curve at 90 degress' solution for a long time now. I just can't believe that there's no better way than to start drawing lines in the view. It seems a bit half arsed to be honest. Also, the hinge line orientation is then not actually related to anything on the model, so is not associative.

HGE, as I said, I'm on NX4...I've not seen an 'Orientated Section View' command. Whereabouts is it ?

John, I know that you can use a planar face, and the axis of a cylinder, but it's a curve I want to use.

I guess I'll put an extra reference line in the sketch, that way at least it's associative to the other geometry.

Cheers for the replies anyway !

Papa.

 

[Spankpapa]

Right, we've figured it out. Not perfect, but it works.

Insert Section View,
Pick Parent View
Pick 'Hinge Line' icon
Scroll down to 'Vector Constructor'
Pick 'On Curve Vector' icon
Select required curve
Change radio button from 'Cartesian' to 'Spherical'
Pick 'Show/Edit Contraints' icon
Remove the contraints shown, OK
Add 90 degrees to the THETA value, OK

Now sit back and admire your work.

Any better/quicker methods, please let me know

Cheers

 

[phillpd]

Spankpapa,

I was hopeful that would also work for a projected view, where you need the hinge line to be 90° to the objects available for selection. Doesn't appear to be associative to the base view though.

And what a pain attempting that process in NX6.



Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[Spankpapa]

Phillip,

I suppose it depends on the objects available for selection I guess. What were they ?

You mean the projected view is not associative to the base view after creation ?

 

[phillpd]

I simply selected an edge and added 90° to the 'Spherical' value.

I updated the model, rotating the edge, but the projected view didn't update.

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[HGE]

Spanky,
I didn't know you were on NX4 when I made my suggestion. The function that I recommended (Oriented Section View) is new to NX6.

 

[Spankpapa]

Phillip,

I tried out what you were saying, and used my method to define the projected view hinge line. When I rotated the base view, the projected view also moved, although I did have to update it.


HGE, no worries, I realise we're a little behind the times here !

 

[phillpd]

Rotating the base view will update the projected view.

But if you edit the model, rotating the geometry you used for defining the hinge line, then the projected view wont update.

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner