Editing Feature Parameter Templates - NX 7.5

[DaSalo]

I'm interested in editing the OOB ASME feature parameter template that controls hole callouts. I can edit things like arrow type without any trouble but what I want to do is change the way the thread is called out from "1/4-20" to ".250-20" . I realize that this is not a standard way to do this and that the fractional format is correct for nominal sizes such as this. I'm trying to make my drawings conform more closely to "the way we've always done it" while still taking advantage of as many of the automation features in NX as possible. Currently everyone here just types in their thread callouts manually so the ".250-20" was the easiest way for them to go about that.

Thanks for the help.

Oh, one more thing. I would like to change the way the depth callout behaves. If the hole is a thru hole I don't want it to add "thru" to the callout. I just want the hole diameter. If the hole is anything but a thru hole I want it to add the depth dimension. I can't remember exactly what the behavior is in NX7.5 currently but I know that in NX6 it would always add "thru". I think in NX7.5 it gives the depth dimension no matter what. So if the hole goes thru a 1.00 plate it gives me a depth of 1.00.

 

[DaSalo]

One more thing, what if I want to go really old-school and have the callout for a screw clearance hole read "Drill and C'bore for .250 SHCS". If the hole was created using the hole tool as a screw clearance hole for a shcs is there way for the software to pull that information and apply a completely customized callout such as this?

 

[ewh]

AFAIK (I don't have the ASME standard available right now) both fractional and decimal thread callout formats are acceptable.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[JohnRBaker]

OK, whether a thread is called out using a fractional or decimal format is not really under the control of the Drafting standard that you're using, but rather which thread standard you were using when you defined the threaded holes themselves. Now it turns out that there are actually 2 different ANSI (Imperial unit) thread standards, the more common Unified or UN-thread format, is specified in fractional inch values and is what's most often used for machine design. However there is another standard, the UNJ-thread format, which is specified in decimal inches. The UNJ-threads (which are available in Normal, Coarse, Fine and even Extra-Fine) are generally used in Aerospace applications, and as such we support them as well and are on the list of standard thread formats available when specifying a Threaded-Hole feature in NX. Now the only issue that you may have with using UNJ-threads is that the sizes are specified to 4 decimal places, not 3 as you've indicated in your example. Now you can either use these UNJ-threads and just accept the extra decimal place or you could take the thread standards table and create a new 'standard' of your own using 3 decimal places.

Anyway, take a look at the UNJ-thread standard and see if that will help.

Now as for actually editing or changing the content of the Drawing thread feature call-out, you could try editing the so-called 'inh' files, which can be found in a folder titled 'inh_files' in the UGII folder where NX is installed. These are 'normal' part files which contains some special formatted 'dimensions' which are inherited into a drawing based on finding certain hole feature types. Now THESE files are defined based on the desired Drafting standard in use and while they CAN be edited there are limitation as to what you can and can not do. For example, you EDIT or DELETE the text that you find there, but you cannot ADD any new text or notes. The reason for this is a long story and it's not somthing which can be addressed easily and therefore has been deferred to a future 'auto dimensioning of features' project which has not yet been fully scoped or funded, so for we're stuck with what we have. Now there's nothing stopping anyone from developing their own NX Open application which could do this, but it would not be trivial if you were looking for something which would be associative.

Anyway, I hope this helps.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[DaSalo]

@ EWH : Your right, both are acceptable. I actually like the fractional format better because it makes it very clear that you are expressing the name of a size, not an explicit dimension that would be governed by title block tolerances or any other tolerances elsewhere on the print.

@ John: Thanks for the tip about the UNJ standard. We are heavily involved in aerospace work but I had never seen explicit mention of that thread standard before. That said, I'm going to stick with the UN standard. The UNJ standard drops the "#" designations, i.e. #10, #8, #6, and expresses those sizes as decimal inch as well. We are all very used to seeing the "#" size designation and I think that would be more confusing than the fractional formatting I was initially trying to avoid. I'm just going to use the callouts as provided and everyone will eventually get used to it. I feel better about that decision now that I've done my due-diligence. If I get some spare time, which has been in very short supply recently, I might make up a customized standard that keeps the # sizes but expresses everything 1/4" and up as decimal inch.