NX6 Drafting Question

[StewB]

Hey guys! I've been using these forums for a while to find answers to NX and other CAD apps, thought it was finally time to create an account.

I'm in the process of transitioning from I-Deas (4 years experience) to NX6. My current contract requires me to migrate old I-Deas data into NX6 using CMM Solo 6. Part and assembly migration went pretty good but drafting not so much.

Anyway, in I-Deas I'm accustomed to adding my own lines onto a drawing sheet, either to aid in dimensioning or create my own customized centerlines. Is there a way to do this in NX? I can create lines, but they never o-snap to objects in my view, even though o-snaps are turned on. I also tried "Sketch on Sheet" but that didn't work either. I have talked to 2 different GTAC reps, one didn't understand why I would want to do this and the other is still "investigating."

Also, if any of you are familiar with migrating drafting sheets from I-Deas, I could use some advice on the "Drawing Overlay On/Off" because it doesn't seem to be functioning properly. GTAC wasn't much help with this issue either.

And finally, when creating a new view, the "Orient View Tool" causes NX to crash with an "Internal Error: memory access violation."

Ok, I'm done for now. Thanks!

 

[ewh]

Have you tried to create your lines while the view is expanded?

The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]

 

[StewB]

Whenever I expand the view, all curve options except for Text are greyed out.

 

[Xwheelguy]

I believe that starting with NX6, the traditional method that veteran NX users were used to using (Expand View, create curves) has been replaced with the Drafting Sketch Tools.

Here's how it works:

Select the view in which you wish to Sketch and make it the Active Sketch View (that's why your Osnap wasn't working, you had another view selected or maybe even the entire drawing sheet). Once you've done that, you can utilize the Osnap icons as well as using Geometric Constraints to lock down the sketch geometry to the model edges shown in the view.

If at all possible, I would avoid using 2D curves in place of Utility Symbols (centerlines). You have your choice of automating the centerlines or manually creating them with the option of using Point Constructors (similar to Osnapping). The reason being is that it's sometimes necessary to add a Cylindrical Diameter Dimension to a detail view and if you have a Utility Symbol Centerline showing in that view, you can dimension to it rather than using the entire diameter of the cylindrical feature/surface and the software will automatically double the radius value into a diameter.

Sorry, but I cannot offer any advice on the Overlay item...I've never used it before.

If you're experiencing memory access violation errors, first try to exit NX and restart it and see if you get the error again. If you do, then try restarting your computer. If that doesn't help, then I'd say it's time to call GTAC and send your NX file into them to see if they can duplicate the problem, if they cannot do it without your file on their own.

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.

 

[StewB]

Thanks for the advice, Tim.

As for the memory access violation, I did try restarting NX but I haven't tried restarting the computer yet. Also, most of my work is classified so sending files to GTAC is out of the question.

 

[Xwheelguy]

No problem, Stew. I hope all suggestions are of some help to you. I've been in your shoes before, but in reverse...I was schooled on UG/NX then was expected to teach I-DEAS to myself, which didn't pan out too well.

I would still try to call GTAC about the memory access violation error, regardless. If they can duplicate the issue, then there won't be a need for your file. Just walk them through the steps you took prior to the error, if possible. However, if you're working on a huge assembly, then the issue might be limitations of 32-bit hardware.

While you may have not had a very good experience with your first few calls to GTAC, do not give up on them...there are some very knowledgeable people that have been working there for over a decade. It's just sometimes difficult to get in touch with those people that would be of most help to you. You can always call back later with the same problem if you're not satisfied with the results. The squeaky wheel tends to get oiled if the squeak is persistent enough. ;o)

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.

 

[hudson888]

If there is something to snap to like and arc centre or a line midpoint or endpoint then of course you could always add those centreline using the drafting "Utility Symbols" tools provided. This would seem a little obvious to most but as you're a very new user there is always the slightest chance that this hasn't been drawn to your attention.

Cheers

Hudson

 

[BOPdesigner]

I was wondering how to do this the other day (sketch/snap to objects in drawing views). So in NX 6, I have set a view as the active sketch view but none of the snaps work. Yet in another view when set as active sketch view, some of the endpoint snaps work but nothing like arc centers, line midpoints, etc. can be snapped to. How do you get it to snap to everything like it would in the modeling application?

 

[JohnRBaker]

OK, on your Selection Bar there is an item titled 'Selection Scope'. If you're working in the Master Model mode, make sure this is set to 'Entire Assembly' and then you will be allowed to select snap points which are part of the model in the view selected.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
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.

 

[BOPdesigner]

There we go. Always a setting somewhere that is off. Thank you John.