Drawing curves in expanded views 1

[xfv8]

Hello all,

Occasionally I need to draw curves in expanded views for the benefit of my machine tool operators. It appears that this functionality is now absent in NX6. Is this now the case and is there an alternative method I can use without having to add curves to the model?

 

[joycejo]

Righ click on the view boundary and select Expand Member View.



John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO

http://www.myigetit.com

NX3,4,5,6 Solid Works, Pro/e, Solid Edge

 

[Xwheelguy]

You can also Sketch on a View without having to Expand the view. We used this method for background geometry of revolved section views that was rotated out of view or skewed after making the section view.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[xfv8]

Thanks for the response guys.

Joycejo: Yep, I have no problem expanding the view, but all the Insert > curve options are greyed-out, apart from Text which can be added.

nkwheelguy: Okay, I can insert a sketch, but I can't constrain it to the edge of the component, the 'old-way' allowed me to infer the curve to say the start point of the silhouetted edge of the component, and any other inferred point, (i.e. a mid point etc.).

 

[xfv8]

NX4 image attached

http://files.engineering.com/getfil...e7-ba53-921bd103d922&file=Inferred_curves.JPG

 

[joycejo]

"Joycejo: Yep, I have no problem expanding the view, but all the Insert > curve options are greyed-out, apart from Text which can be added."

Wow that's wierd. If you activate the curve toolbar you can select them from the icon, but the insert curve option is greyed out. Looks like its time for a I.R.

I will check NX6.0.3 on another computer later.

John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO

http://www.myigetit.com

NX3,4,5,6 Solid Works, Pro/e, Solid Edge

 

[joycejo]

OK I did some checking and the Insert - Curves option, When your in drafting creates a sketch and you can;'t create a sketch in an expanded view.

When you expand the view you have to use the curves icon and you can activate the Lines and Arcs toolbar.



John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO

http://www.myigetit.com

NX3,4,5,6 Solid Works, Pro/e, Solid Edge

 

[hudson888]

It seems to me that all you need to do is turn on the curve creation toolbars in the drafting application. One you expand the member view you can add curves, section curves, or basic curves to your heart's content.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Xwheelguy]

xfv8,

I'm not sure why it won't allow you to do that. Granted, I haven't used NX in a few months, but the last time I did you could geometrically constrain to view geometry/edges. You may have to physically apply the coincident constraint to achieve this for one reason or another.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[xfv8]

Gents,

I tried inserting curves by turning on the curve creation tool-bar as per joycejo and hudson888 suggestion, it now allows me to add curves as per NX4 as intended, so thank you all for that. I still think it should be investigated as to why it doesn't work via the menu - a task for Mr. John R. Baker presume?

nkwheelguy, the only constraints offered were fix and fix-all. Thanks for trying anyway.

 

[Xwheelguy]

Hmmmmm. Something isn't sounding correct here in regards to the Sketch route. I bet you're sketching on the Drawing and not the View. You have to select the View, make it Active THEN Sketch (if I remember correctly).

I'm positive that Sketching on a View did work at one point in time because I used it on Section Views where geometry that was rotated out of view could be created via a Sketch & if the model changed, the sketch would update accordingly.

I used the same method you're using (Expand View -> draw curves) up until the Drafting Sketcher came along and allowed me to attach curves to the model edges in the view. Once I saw that the Sketch curves would follow the model edges via the constraints, I went the Sketch route permanently. Not trying to beat a dead horse here, just not sure why it's not working for you in this instance.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[xfv8]

To nkwheelguy.

Ahhh...that's got it working; the penny dropped when you stated that the trick was to make the view active, which was something I was not familiar with being a CAM guy. I also now appreciate the use of using sketches to maintain the associativity in drafting, I do use sketches in CAM world when I create boundaries for constraining a machining area.

Thanks for the tip, & regards from 'across the pond'.

 

[JohnRBaker]

The reason for the 'issues' with the 'curves toolbars' is because we would really prefer that you use the new 'Sketch in View' approach, so while it's still possible to create non-sketch curves in the views, as some have found out, we didn't want to make it too easy then no one would try out the 'Sketch' options. ;-)

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.