Position of tolerance in association with the dimension

[Nick66]

Hi,

I'm working with Nx8.5. While in Drafting I go to: Preferences/Annotation, I select tolerance and then chose "Upper Right" from the drop-down of "Alignment Position". Now I create a dimension with a +/- tolerance and the tolerance is still defaulting to being directly to the right of the dimension instead of to the upper right of the dimension where I need it to be. I have also tried the same method after creating the dimension, left clicking on the dimension and bringing up the Edit function. Is there something that I am missing that I need to do?

Any help in this matter would be greatly appreciated. Thanks in advance.

 

[ewh]

I always thought that alignment position refered to where the text as a whole is placed relative to the cursor position.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[Nick66]

I need to place the tolerance to the upper right of the dimension. If I am not going about doing so in the correct way please tell me the proper way to make this happen.

 

[cowski]

Are you working to a particular drafting standard?

www.nxjournaling.com

 

[Nick66]

I work for a large U.S. manufacturer of solid round cutting tools. If you are familiar with the NAS 986 (which is in no way intended to be a drafting standard) and you look at the formatting, when you see toleranced example dimensions their tolerances are always slightly smaller and to the upper right of the dimension. This is not an uncommon practice (at least within the U.S.) as I've seen this done often throughout other jobs I've had. I was also able to do this easily with Nx4, but that was a little while ago... I cannot be 100% sure of exactly how it was achieved.

 

[ewh]

Search the Help files for Symbols and Text Control Characters.
Among them is Superscript <H>, which will place a half-size character above the top line of the text. Use <H> at the start and at the end of the characters to be superscripted.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[Nick66]

ewh, I'm really not sure you are getting what I mean. It is really quite simple.

 

[JohnRBaker]

Perhaps an image of what you're looking for might help...

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Nick66]

Thanks John, please see the attached

 

[Arkance/PhoeNX]

Attached video shows how to do it in NX8.5.
I did a quick test in NX4 and can't do the same, so I'm not sure how you did it.


Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[JohnRBaker]

That's still not giving him what he wants as it doesn't work with a '±' tolerance.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Arkance/PhoeNX]

you're right John, I forgot about the '±'.
Only other way I can see it being done in NX4 or NX8.5 is to do it as appended text.


Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[MickyV007]

Please have a look at the attachment. First place dimension without tol, then goto edit annotation and use <H>$t.005<H> for uppercase.

Best regards,

Michaël.

NX7.5.4.4 (NX8.5.3) + TC Unified 8.3
Win 7 64 bit

 

[Nick66]

Thanks MickyV007. That is precisely what I am looking for. Can you please let me know how to adjust the spacing between the dimension and the tolerance? In your attachment the tolerance is much closer to the dimension (which looks right to me). If you see my attachment here, they look a bit far apart.

 

[cowski]

Be aware that MickyV007's method will result in a dimension with manual text; this means the value of the dimension will NOT update if/when the geometry changes. You have been warned!

www.nxjournaling.com

 

[Nick66]

Thanks Cowski, I do realize this. If there is a way that you know of to achieve my desired result as "tolerance" instead of "appended text" please by all means let me know.

 

[ewh]

This may or may not work, seeing as you are already aware of the text control characters ;-)
<Gr> where r is the spacing factor relative to the current spacing

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[ewh]

Of course, that does not solve the associativity issue...

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[MickyV007]

Or just place a space between 12 and <H>

Best regards,

Michaël.

NX7.5.4.4 (NX8.5.3) + TC Unified 8.3
Win 7 64 bit

 

[cowski]

NX does not fully support the style you desire. The best course of action is to use what NX offers and open an 'enhancement request' (ER) with GTAC. You will get the full benefit of what NX offers and you may get the dimension style you want in a future release.

If you are really stuck on this dimension style and simply must use it now, I suggest creating the tolerance as a separate note and using the 'origin' tool to associate it with the dimension (as the dimension moves, the tolerance note moves with it). It will look like your example, but you may lose out on some functionality (if any downstream functionality queries your drawing dimensions they won't pick up on the 'tolerances' that you have added, but the dimensions themselves will be fully associative to the model).

www.nxjournaling.com