Cosmetic Threads in drawing not completely shown

[DMiller01]

I am currently using version 6.0.2.8 with XP professional. When using the hole function to create threaded holes the cosmetic representation of the thread in my drawing only shows 270 degrees of the thread diameter. I also find that sometimes using "feature parameter" to place a callout of the thread in the drawing that the thread specs show up but the tapped hole size does not.

Has anyone had any similar experiences? Is it a version bug?

Thanks

 

[jerry1423]

I have given up as far as using "feature parameter" for tap dimensions ... I guess it will be better in NX7.
Are you speaking about the top view of the tap? If that is that case then change the type of representation that is being used:
rmc (right mouse click) on drawing view > style > threads > thread standard > change between the ISO and ANSI styles (and press "apply") and see if that helps

 

[jerry1423]

Sorry, I didn't initially look at the picture you had - you just have to change the thread representation and that will fix it.
Did you use "feature parameters" to dimension the tap in that picture? It looks better that what I got, maybe because I have metric holes?

 

[DMiller01]

Thanks Jerry. I changed the standard from ISO-Simplified to ANSI-Simplified and that took care of the problem.

 

[DMiller01]

Jerry,

I did use "feature parameters" on this thread but you can see that it did not include the tapped hole size which I'll have to add in manually.

 

[JohnRBaker]

When you say "tapped hole size", are you talking about the size of the tap-drill itself?

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.org/museum/

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

 

[DMiller01]

John,

Yes. The callout for the tapped hole sometimes will not display. In the Feature Parameter dialog I select both the hole icon and the thread icon for the threaded hole feature. I have attached an image of the dialog box.

Most of the time it works and displays a separate callout for the tapped hole and for the threaded feature but occassionally I can only get the callout for the threaded feature.

 

[JohnRBaker]

If the result is random that makes it harder to pinpoint. Are you using the same Drafting Standard for each case? Are some of the drawings older and some newer? Are some created using a Drawing template and some not?

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.org/museum/

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

 

[DMiller01]

John,

I will have to start paying more attention to the circumstances where this happens. We have only been using NX for a little over a year and have been using the same drawing standard for most of that time. Most of our parts are created from a common template part that includes the drawing. I'll gather more info and post back with what I find.

Thanks,

 

[JohnRBaker]

The reason I'm asking is that when you created and saved the Drawing template file, it would have been based on whatever was your Customer Defaulted drafting standard at the time, which also would include which 'Annotation Template' is to be used when creating automatic feature annotation.

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.org/museum/

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

 

[DMiller01]

I have found that if I add a hole I can use the feature parameter function to add a callout for the thread and tapped hole in the drawing.

I then delete the call outs and instance that threaded hole to make a pattern. If I try to use the feature parameter function after instancing the threaded hole, I get the thread callout but not the tapped hole call out.

If I delete the instances I still can not get the tapped hole callout to show on the original threaded hole feature.

What does work is if I use the feature parameter function right after creating the first threaded hole. I do get both call outs and I can then instance the threaded hole and the callout remains.

 

[JohnRBaker]

OK, try this. If you know that you're going to want to 'instance' the holes, rather than creating a hole and then instancing it, create instead a point on the face where the hole is to be placed. Then using...

Insert -> Associative Copy -> Instance Geometry...

...create the desired 'pattern' of points (which represent where you wish for your threaded-holes to be).

Now when you go to create your Threaded-Hole, when asked to 'Select planar face to sketch or specify points', with the 'Curve Rule' set to 'Feature Points', select any one of the points, set your desired hole specifications and hit OK. And if you wish to change the number of holes, just edit the quantity value used in the Instance Geometry feature.

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.org/museum/

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