threaded hole: inherit ANSI feature parameters onto ANSI-MM Drawing 1

[potrero]

A long time ago, I posted this question but got no answers ( thread561-225709 ). If anyone has a tip on how to get this to work, I'd appreciate it. We create parts and draft in metric, but often, we have inch holes and threads. It'd be very useful to be able to put the inch spec on the drawing sheet, which is otherwise a metric print.

"I have a metric part with an English threaded hole. When creating a metric drawing, how can I inherit the proper threaded hole callout onto the print (ie: 1/2-13 x 16mm or similar)?

I have tried using the "Feature Parameters" tool, but the thread callout comes in as "1/2 x 1.95" as in 1/2" x 1.95mm pitch...

When using the Feature Parameters tool, selection of the standard "ansi" option is greyed out, leaving only "ansi-mm", "iso-din", and "jis".

I'd appreciate help on this. Thanks."

 

[dpackard]

I was able to reproduce the exact same thing in NX 6.0.2.8

I do not know what is causing this. I will ask around...

Enclosed is the file I created.

 

[potrero]

@dpackard - any solutions?

 

[dpackard]

It seems that there are little to no plans to fix it. From another forum a guy said...

"In june of 2007 I had pulled out a pr out on this problem and I don't think it is fixed yo the pr # is PR5768789"

"I don't know if they are ever going to fix it because they changed it to an enhancement and as of March 14 2008 they have not reviewed it yet."

That is all I could find out.
dpackard

 

[cmacca]

We had the same issue. Metric part with inch holes. There is a utility to change a inch prt file to a metric prt file. Use this to save the inch inh file that defines inch thread callouts to a metric file. Now if your inh files for metric and inch threads are in the location the feature parameters commands looks to you should have a pull down list to choose either a metric or inch template

NX 6.0.1.5, TC 2007

 

[potrero]

@cmacca - this sounds interesting; when I get a chance I'll try it out. Did it fully resolve the issue for you?

 

[potrero]

@cmacca - wow, that's such a great tip! it totally works... Star for you.

for anyone else who has run into this problem, here's a little more detailed description of how to enable the ability to Inherit Inch thread annotations onto metric drawings:

1. Locate the part, "the part ansi.atp.prt" (by default found in the UGII/inh_files directory)

2. Make a copy of it; rename it something like "ansi_converted_to_mm.atp.prt" or anything just as long as the bit "atp.prt" at the end stays intact. (This is necesary for NX to recognize the part as an Annotation Template).

3. Use the utility ug_convert_part.exe (by default found in the UGII dir) to convert this new part from inches to mm.

4. You should be set! Now, when you want to Inherit Inch thread feature annotations onto a metric drawing, you can simply select the part name you gave above, from the drop-down of available annotation templates in the Inherit tool, and it just works.