Attaching a GD&T Symbol, NX3 2

[jackley]

Does anyone know a way to attach a GD&T feature to a side view of a cylinder? The top and bottom of this cylinder needs a flatness and a parallelism spec, but in order to attach to it, I need to create a line. Otherwise I cannot grab anything to attach too.

I have linked a sample image, any ideas? I've looked in the quick pick tab, but nothing can be selected.

Justin Ackley
Design Engineer
jackley@gmail.com

 

[ewh]

Could you add a reference cylindrical diameter dimension and tie into that?

 

[Xwheelguy]

I'd call GTAC about this, unless it's conflicting with your chosen GD&T standard (ANSI, etc.). However, I suspect it's the method used to display the view in drafting....expand the view and rotate the cylinder...see the semi-circular edges? That's probably the culprit. I really despise some of the view methods NX uses...probably why there are so many problems trying to translate a drawing....they're never FLAT like they probably should be.

I tried to use Simplify Curve to "explode" either end of the cylinder and that completely removed the center portion of the ends. Can you attach the GD&T leader to the dimension's extension line instead? How about making a section cut of the cylinder instead of a viewport?

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[jackley]

Well I looked around for adding the GD&T to a dimension extension line, but I can't find anything. I knew about the section view, it does work well there. I guess that'll be my fix for now.

Justin Ackley
Design Engineer
jackley@gmail.com

 

[Xwheelguy]

I hope I can explain this well enough that it's simple....

To attach a GD&T callout to an existing dimension extension line, type your text in Annotation Editor then on the Annotation Placement toolbar, select either of the last 2 pulldown icons on the far left (leader type?). Next select the Leader Tool icon to bring up the Create Leader dialog. Next, select the Leader Type pulldown and pick the 3rd icon from the bottom on the list. Select an existing dimension line then drag to place the callout.

That may not be what you're looking for, but that may be an alternative.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[jackley]

Well this brings up a question. The way you explain it (and hopefully I followed it correctly), it creates the GD&T symbol just like Datum A in the picture on the first post.

Ok, from there, is that the correct way GD&T should be placed, or should be off an extension line, like the flatness and parallel callouts, are?

I am assuming NX will limit me to what is acceptable in the GD&T world and not let me create something that is no longer standard.

Justin Ackley
Design Engineer
jackley@gmail.com

 

[ewh]

There is a leader toolbar which allows you to choose what type of leader you need. Per the current 1994 standard, datum identifiers have a triangle instead of a leader (as shown in your example). The feature control frames are still attached directly to extension lines (as shown in your example) or to a surface or extension line via a leader with a standard arrowhead. NX will let you mix and match, resulting in something not necessarily per the standard.

 

[Xwheelguy]

Justin, are you following any certain standard? If not, then you should (and I emphasize should because I'm not positive myself) be able to use EITHER method (yours or mine). Since we're not able to pick the circular ends of the cylinder, the second method I suggested is the only way that it can be done (in NX) without picking any parts of an existing dimension.

Regardless of what the leader "head" (either a triangle or just an extension line) looks like, it means the same thing as far as I know.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Agriego]

The problem also exists when trying to add ID balloons to a view as well. If the part is cylindrical or has a curved profile, you won't be able to add an extension line leader even though the edge may appear straight. That's been a gripe of mine for a long time. I've been adding a small line segment in the drawing view to allow me to create the leader. Not the best solution, I'm sure, but it works.

Al Griego
Design Engineer
agriego@sj30jet.com

 

[ewh]

Unless you are using associative parts lists. Then you would have to add the line in the component part to ensure proper pl updating (which is a no-no @ sino if I remember correctly).

 

[fred2002]

If you want to have an arrow pointing at 90 deg to the end surface, try this:
1. Create another horizontal dimension, as if you were adding another length dimension.
2. Edit the dimension by right-clicking on it.
3. Change placement to arrows out and drag the number in the dimension to either left or right of one of the flat faces.
4. Right-click again and choose style, then the dimensions tab. Depending on how you selected the edges, click the leader and arrow at one side under the tab headings. Then click apply. The dimension you just created will now lose a leader line and an arrow.
5. Now the naughty bit. From the top menu, select edit > text and then click the dimension (in your case 62). You can now edit this by clicking on the 'A' just above the box.
Select the GDT Symbols box. Delete the 62. Click OK whenb the warning box comes up and enter the desired geometric tolerance. When complete, click close.
You can now drag the tolerance to where you need it.
Repeat the process for the other tolerances you require.
Note that you may need to fiddle with the dimension's style preferences go get it just right.

This may sound very involved but once you've got the hang of it, it's quite easy to do and edit. Beware that it will flag up as a manually edited dimension if you use that particular check.

Hope this helps.

Fred.

 

[Xwheelguy]

That sure is a long route compared to attaching it to a dimension's ext. line.....

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[ewh]

I was thinking the same thing...

 

[fred2002]

I know what you mean. But this way allows the tolerance to stay associative to the geometry (unlike a line in expanded views) and doesn't rely on having an existing dimension in the right place (if adding to an existing extension line).

I tend to find this method more flexible and posted it as a useful alternative. You still have to make sure that it complies with whatever drawing standards you're using, of course. I wanted to post an image of the result that I get, but haven't got an accessible website.

Regards.

Fred

 

[ewh]

Fred,
Try

http://www.putfile.com

Easy to use, and I've had good luck with them.

 

[fred2002]

Thanks for the link, ewh. I hope this works

 

[fred2002]

Oops, clicked submit instead of edit!

Got there in the end!

Fred