NX7.5 Leading Zeros on Drawing Dimension

[jerry1423]

We have been working totally on NX7.5 for around a week now, we moved up fron NX6.
It was just pointed out to me that the leading zeros do not appear on the draawing dimensions, as they did in NX6.
I looked at our customer defaults, and the Preferences, and in all cases leading zeros is checked on, as shown in the picture.
The leading zero dimensions show up fine when opening a drawing in NX7.5 that was completed in NX6.
Is there any other setting that affects the leading zero other than what I am showing ?
Has anybody else seen this behavior ?

 

[jerry1423]

I did discover that leading zeros works fine on the metric dimension, but not the dual inch dimension.

 

[looslib]

That IS the standard for your settings. Inch dimesnions do NOT have leading zeros before the decimal point, only metric dimensions do.

ASME Y14.5M-1994 section 1.6 covers Types of Dimensioning
1.6.2 Decimal Inch Dimensioning. The following shall be observed where specifying decimal inch dimesnions on drawings:
(a) A zero is not used before the decimal point for values less than one inch.

Siemens has worked hard over the years to be sure that they follow the drafting standrads.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jerry1423]

I agree with those standards, but some people here do not.
I just wonder why showing the leading zero on an dual inch dimension worked in NX6 when technically it shouldn't have.

I just wish we'd get away with from dual dimensioning here and everything would be fine.

Thanks

 

[looslib]

If it worked in NX6, I would guess it was a bug.

I thought there used to be settings for secondary dimensions as opposed to primary dimensions. That may have been prior to NX using a GUI to edit the standard settings.

When we converted to UG V10 in 1994 at a prior company, I implemented the setting for metric dimensions NOT using trailing zeros. Talk about a lot of hassels and extra meetings. The company had been on UG for 8 years at that point and had used trailing zeros for the default tolerance, like they had done with inch dimensions. When drawings started being regenerated with no trailing zeros on metric dimensions it all hit the fan. I held my ground and engineering changed their practices because we sated on the drawing that our drawings complied with ANSI Y14.5-1989 (I think it was), at that time. By the time we switched to Pro/Engineer in 2003/2004 it was a non-issue.

We did not dual dimension the metric drawings, but we had a GRIP program that would scan the drawing for all dimensions and put them in a reference table on the drawing edge showing all metric dimensions and its inch conversion.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

Someone probably complained that we were not in compliance with the ASME standard and so we 'fixed' the problem.

That being said, you can override the 'standard' by opening your Drawing templates (the actual master template files) and going to...

Preferences -> Annotation -> Units

...and setting the 'Zero Display' options that you wish. Now save the template files and you should be good-to-go.

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

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

 

[jerry1423]

John,

I toogled leading zeros on, but it does not affect the dual dimension.
so the "overwrite" thing that you mention works, but only for the primary dimension.

On our drawings we have milimeters as the primary units, and inches as the secondary units.
So an example dimension would look like this: 15.00 [.5906], with leading zeros on.
But when I change the primary units to inches too, the dimension looks like this; 0.5906 [.5906]

This issue would not be that big of a deal, because the dimensions can be changes easily after opening them up in NX7.5, many of them change automatically, but double-clicking on them will force them update.
but the problem comes in when the manually added numbers, such as GD&T tolerances all need to be edited manually.

 

[JohnRBaker]

I think this issue has been discussed before (but it might have been in som eother forum) and at the moment this is not supported.

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

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

 

[looslib]

By going against the standards you are creating more work for yourselves. As for Siemens 'fixing' the problem to make it easier to violate the standards, I would not like them to invest any time doing that. They have spent considerable time making NX drafting conform to the various standrads that they do support. Building kludges to circumvent the standards should not be done.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jerry1423]

I hear ya . . . If it was up to me I'd follow the drafting standard tightly, but this is not up to me. Lots of old guys working here, who follow antique company standards.
I like the way NX follows the standards . . . it drives me nuts sometimes to see drawings done in AutoCAD, or similar system, with no regard to standards.

 

[looslib]

Sometimes, you just need to sit down and explain why you need to make the change.

In another forum, there is a similar discussion. I asked the guy why they wanted trailing zeros on metric dimensions. His only reason was that was how it had been done. When I pick up a print and quickly scan it to get an appreciation of the size and I see 20.00, I assume the print is in inches. When I see 20, I assume metric. Big difference in part size between 20.00 inches and 20 millimeters.

Standards are created to reduce errors and ease communication. We may not always agree with them, but if we agree to follow them by noting that on our print, then we should follow them.

Jerry, I am not picking on you directly. You are in the choir chairs with me. We need to sing louder is all!


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli