Truncating/Folding Linear Dim Extension Lines

[MCGNX]

How can it be done succesfully in NX5?

I have a detail view of a revolved cross section and love the fact that you can dimension across views to get the real dimension and keep associativity with it. However I can't find a way to truncate or fold the extension line besides flat out turning it off, which doesn't look so hot. Is there a way to do this?


Also while we're at it, is there a way to center the entirety of dimension text (including tol's and appended text) between the extension lines?

 

[JohnRBaker]

Can you provide a 'picture' of the desired results?

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/

 

[hudson888]

MCG,

Okay for the first part I don't know what your getting at. If you could provide a small JPEG with a mark up then that would be good. There are different dimensioning and extension line styles available under the style settings, and also if you don't want to trawl through the whole thing get close by opening the relevant dialog then hit F1 which will bring up help and probably list all the available methods, you may find it in there for yourself.

Now as for centering the dimension especially using the automatic dimensioning method they will snap or at least subtly hesitate as you pass by the central point between the two extension lines either when you edit the origin or during initial placement. For methods other than automatic this isn't necessarily the default position but you can still notice the hesitation and manage to make a central placement. Apart from that another possibility maybe that you just want to alter the text justification which you should be able to find using the style settings. You'll be looking for three standard icons for left right and center familiar to users of Word and other office software. Other settings to do with line spacing and gaps between text are set under lettering, using numeric values.

Best Regards

Hudson

 

[MCGNX]

Here is what I'm talking about


The centered dims are just a minor annoyance, but I do think they look better centered. The detail dims however, the only way to succesfully do it is to dimension to a drawn line, then override the dim text. This option is pointless to me because you lose the dimension associativity to the model. Another way is to just suppress the dim lines which leaves you with what you see on the far right. Another way I've tried is to suppress the dim lines and then put in a note with a leader so it emulates the dimension I am trying to get. This doesn't work so hot either because the leader does not move with the line, and it is difficult to align. Also, if you associate the origin to the dim, only one end of the leader will move with the dimension. Now another way I have tried is to put in the original "true" dimension as shown and suppressing all the dim lines, then putting in a dummy dimension line with the dimension text removed. You can align the dummy dim to the "true dim" text horizontaly, but not vertically....which means the gap does not move with the dim but the ext. lines do. This also allows the dim to be centered (again, just a minor annoyance) but is a pretty painful process to do.

Just wondering if there is an easier way.

 

[hudson888]

MCG,

NX nor any other CAD system I have seen does not appear to support this really well. I can do it but it is neither very easy nor straightforward, and I would not at the end of the day want to use this method. But I made something work.

You can dimension diameters to a centerline by first creating a symmetrical centerline as shown in the attached images. For multiple diameter dimensions to a theoretical straight line in space you'll get away with this. to make it work I created a second detail view with the centerline but with no reference circle or letter on the main view, and added the symmetrical centerline to it. Add the dimensions change the arrow type and ditch the extension line on that end. Then convert that view to reference so it does not show up on the drawing. You can even blank the centerline to complete the effect.

One note that I found in this was that the reference view printed out on a PDF using the printing from graphics window method and that should not be the case, better to just manually edit the boundary to a small rectangle that doesn't cross any of the geometry.

Yes it is a fudgey way of going about it, you probably won't like this very much, and nor would I bother. However the good news about it really is that I came up with the technique and images within 5 minutes of deciding to try so although inelegant it could hardly be called painstaking.

Best regards

Hudson

 

[uwam2ie]

I found no solution for truncating Dim, there's something on radial dims. Or ?

 

[ewh]

I've used a method similar to hudson's in the past. Easy to do if you need it.
Add a duplicate view (a detail view requires more effort to get right, turning off labels and such), create a centerline along the axis in question, dimension to it as hudson suggests, then change the view bounds so that nothing shows. Turn off the extension line at the axis.You can then move this view wherever you want, and the dimensions will be maintained.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]