Default tolerence for global NX modeling 3

[mhrub]

Hi,

I was just wondering if anybody knew how to set the standard tolerance in NX 7.5 for tools such as (but not limited to) projecting curves, making chamfers, and section curves. Normally these tools default to .001 but I would like to make it at least .0001.

Right now I am manually putting in .0001 every time I have to use a tool that has the tolerance setting. I was wondering if there was a place in customer defaults or somewhere else that does this?


Thanks in advanced,
Mike

 

[JohnRBaker]

First off, you only have control over a single default value which is applied to ALL modeling operations. There are NO user-settable defaults for individual feature types, just local settings at the time that you're creating the feature.

So, if you wish to change the global tolerance value used by Modeling, go to...

Customer Defaults -> Modeling -> General -> Tolerances/Scales

If however, you wish to only change it for the Part file which you're currently working on (noting that these changes ONLY effect new features created and has no impact on features already in your Part file), go to...

Preferences -> Modeling -> General

...and change the Distnace and/or Angle tolerances.

That being said, WHY ARE YOU SO INTERESTED IN CHANGING YOUR GLOBAL TOLERANCES?

What do you expect to gain with these smaller tolerance settings?

Are you creating very small models with very small features using very small dimensions? By small, I mean overall sizes of less than an Inch or two.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
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Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[mhrub]

John,

Thanks for your reply.

The second method you gave me does globally set the tolerance within the part, however the first method (which I would like the most) about setting the default in customer defaults does not appear to be working.

With setting it in customer defaults, when I make a new part it should default to say .0001 instead of .001, correct? For some reason it shows in customer defaults that it is 1E-4 however always defaults to .001, unless I use option number 2 and always set it in the part.

I am working on airfoil sections with tolerances that have tolerances within 10ths therefore having a section that is within .001 does not work very well. (for instance)

Thanks for your help,
Mike

 

[cowski]

Are you starting your new files from a template? if so, your new parts will inherit the template part's settings. Changing the customer defaults only applies to a new blank file. Open your template file(s) and change the desired settings; your new parts will now reflect your changes.

www.nxjournaling.com

 

[Toost]

Reading what your task is, the airfoils. I dont want to "write anything on your nose here", but...
Be careful, i have been discussing aero and hydrodynamic surfaces with a number of companies/ users, and very often they tend to believe that their input data is perfect and will produce perfect curves and surfaces. Quite often the input data came from FEM / CFD analysises, which by nature is a rough estimate. Also the input data often is way too dense to be able to map 1/1.
Then to use that data with very small tolerances will produce completely un-usable models. I have a, lets call it, "wing" in an NX part, it's ~6 mb and it only has two faces ( Surfaces) and it is completely un-usable. - Way too much data in these two surfaces.
In this case , the less input data the smoother surface...

Regards,
Tomas