Thread hole leader note 1

[Michel1978]

I found an old thread about this, see thread561-102354.

That doesn't work for the new hole/thread command, from NX5.

Is there any way to fix this problem?

I use NX5.

 

[JohnRBaker]

I just tested this with NX 5.0.6.3 and it worked fine, Note that when you get to the point where you are asked to select the 'threaded hole' feature, you will be presented with TWO features, you need to select the SECOND item with the icon with the 'threaded' appearance.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[Michel1978]

You are right. I know now why it didn't work. I had turned on the chamfer when creating a threadhole. The chamfer was just the same size as the thread, hence NX didn't recognize the thread in the drawing.

But where can you set the style of these annotations, because they are different from my other dimensions.

I use NX5.

 

[JohnRBaker]

The style of the 'auto feature dimensions' are controlled by a series of templates which can be found at...

...\UGII\inh_files\

...and the actual file being used is set in Customer Defaults at...

File -> Utilities -> Customer Defaults -> Drafting -> General -> Standard -> General -> Miscellaneous

...where you enter the first part of the name of the template file you wish to use.

If you wish to customize the actual template files, you can do as well by copying one of that close, make your changes and giving it a new descriptive name and referencing that file instead in Customer Defaults.

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

 

[BEAEROHEAD]

Use the hole function to create holes.
Then Insert/Feature Parameters. Look for the feature in the list. Select the hole to dimension/Select the view to put the dimension in and apply.See attached

 

[hurley710]

Nice feature. Never used it before today as I always have re-entered the line callout manually. Only question for me is can you have it dislay the thread callout (i.e. 1/4-20 UNC - 2B)?

 

[BEAEROHEAD]

Yes it will call out the treads as well. It extracts the hole data whatever it is.

 

[potrero]

On a related note, one of the things I sometimes run into is the situation where Inch holes are needed in an otherwise Metric part. The problem arises in that if you are working in a metric drawing and attempt to use the "Feature Parameters" functionality in Drafting to pull in the thread callout (say, "1/4-20 UNC"), you instead get something like "M 6.4". There's a drop-down menu in the Feature Parameters command block to select drawing standard, but ANSI-Inch is greyed-out.

Any suggestions?

 

[BEAEROHEAD]

As long as you use the hole function and the thread function, it will extract metric or inch data.

 

[potrero]

beaerohead,
Here's what I have observed:
The part in question is a metric part, with a threaded hole, 1/4-20 UNC, created using the 'new' Hole function.

Option 1: Create Metric drawing of the metric part, then use "Feature Parameters" to create an annotation (selecting the 2nd Threaded Hole feature corresponding to the actual threaded hole, not just the thru drill). The annotation reads "M 6.4". Looking at the Template drop down menu in the "Feature Parameters" block, one can see that only "ansi_mm", "iso_din", and "jis" are selectable; "ansi" is greyed out.

Option 2: Create Inch drawing of metric part. "Feature Parameters" results in successful annotation "1/4-20 UNC-2B". (Actually there's an issue in that the depth is falsely reported as a value when it should read THRU, but that is another matter...) As a note, the Template drop-down menu now has only "ansi" as the selectable option; the others are greyed out now.

So, unless there is a setting where I can enable "ansi" templates inside a metric drawing, and the other templates inside an inch drawing, then it would seem that the problem exists as I've described it in the above post.

Where's that setting?...

 

[BEAEROHEAD]

(NX5)when assinging a thread to the hole, it gave me an option for metric or inch. (see attached) Hope this helps?

 

[potrero]

In NX6.0.1.5 MP1, you don't have to add threads separately to holes; it's part of the hole dialogue. See the attached image.

 

[BEAEROHEAD]

Thanks for the tip. In searching NX5 can do the same.
( I am a newbee to UG )

 

[JohnRBaker]

Due to architectural limitations, you can't reference a template file created in Imperial units with a Metric drawing or a Metric template file by a Drawing file created in Imperial units, which is why we prevent you from even attempting it. However, I think I might know a way out of this conundrum but I'm going to have to do some experimenting first, however if I learn anything I'll let you know and if it works I might have a solution that I'll be able to share with everyone.

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

 

[potrero]

thanks John, appreciate your trying to help resolve this.

 

[BOPdesigner]

John, on your post above with the path to see which inh_file is being used for the feature. I follow to:
File -> Utilities -> Customer Defaults -> Drafting -> General -> Standard -> but on this Standard tab I don't see another General -> Miscellaneous. Only the Miscellaneous tab at Drafting General. And this tab does not show which inh_file is being used.

 

[JohnRBaker]

My experiment was partially successful. I can fix most of the issues with respect to Simple, Counterbored and Countersunk holes, but I can't quite get the threaded hole call-outs to work correctly when automatically annotating an Imperial threaded hole in a Metric part or vice versa. Sorry. And before you ask, the solution to that last part would require a significant project to be funded in the Drafting group which puts this way out of reach as a simple PR.

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

 

[hudson888]

John,

Why not bundle it in with the PR to support Whitworth threads. Flogging a

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

As for the question about setting which template file to use, you have to go down one more level as these are assigned a per drafting standard basis.

OK, when you're where your picture showed you to be, go back and select the 'Standard' tab (upper-left corner) and then select the desired 'Drafting Standard' and then hit the 'Customize Standard' button, which will drop you into a sort of mini-Customer Default just for setting up your drafting standards. Now go to THAT General page and select the 'Miscellaneous' tab and you'll find what you're looking for.

Note that any changes made while in this mini-Customer Default will have to be saved as a new standards file (technically you don't really want to override an existing standards file and we make it very difficult to do so) in order to be able to use any of the changes that you've made.

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

 

[BOPdesigner]

I edited my inh_file and still no luck with a filled arrowhead when inserting a feature parameter. Contacted GTAC and they created an ER.