Threaded Hole in NX6

[scottpainter]

Please spare me the rant about NX6 being old, unsupported, etc. It's not my decision to still be using it...

That being said, I have created threaded holes in a part using the threaded hold feature or command in NX6. In NX7 and NX8, the holes always had a dashed circle around them on the surface that is pierced by the hole. I see no such circle on the solid model in NX6 nor in the corresponding view in drafting. When attempting to use the "Feature Parameters" command/feature in drafting to annotate the hole, all I get is a diameter. No depth, thread, etc. Our parent company has this system pretty locked down and customized so I'm assuming it's got something to do with them, but thought I'd see if anybody out here can help.

 

[soudekerk]

did you check in the drawing using the VIEW STYLE under THREADS that you have ANSI/Simplified one and its not set to none??

Scott A. Oudekerk
BorgWarner Morse TEC
Ithaca, NY

 

[scottpainter]

Yes, but thanks for the suggestion.

 

[JohnRBaker]

Can you provide a sample NX 6.0 part file with a threaded hole where you're seeing this behavior? The reason I'm asking is because I can't reproduce this problem using my copy of NX 6.0.

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.

 

[scottpainter]

If you're not seeing it, then I'm fairly certain that it's due to my parent company across the pond running the admin of the software and customizing all defaults. We aren't running TCE either. Using Agile PLM so I'm not sure how to export it other than doing a 'save as' to local directory. How should I deliver it to you once I figure it out? Attach it to this thread? I'll include the drawing too since I'm guessing if you put it in an out of the box NX part file, it will work just fine.

 

[JohnRBaker]

Doing a Save As is fine. Yes having both the part file and the drawing would be better. Just do a Save As on both files, zip them up and use the 'upload your file to ENGINNERING.com' option at the bottom of the page.

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.

 

[scottpainter]

Here you go. Thanks for looking into it.

 

[scottpainter]

BTW... same thing happens with counterbored, countersunk, any hole... all it does is put in the diameter, no CB, CS, depth data or anything.

 

[JohnRBaker]

OK, select your Drawing views, press MB3, select 'Style'. When the dialog opens, select the 'Threads' tab and change the 'Minimum Pitch' setting from 0.050 to 0.000 (which disables this function). Now if you're using a Drawing template you need to open that file and select...

Preferences -> View...

...and then follow the steps above and then save the Drawing template file.

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.

 

[scottpainter]

Thanks for the help. I was able to get a solid line to appear around the tap drill hole in the part now and able to get M4 to show up when I try to use Insert--Feature Parameters now. But there's still no depth component to the M4 callout as there was the last time I used the feature. Maybe it has something to do with the fact that I'm working with ISO rather than ANSI now? I would like to see it show something like M4 x 8<#D> so that I don't have to go back to the model to look up the depth of the hole or thread or cut a cross section in the drawing just to show the thread and tap drill depths.

 

[scottpainter]

Also, the solid line around the tap drill hole is usually a dashed line. Can't figure out why it's solid.

 

[scottpainter]

Well, since you're on PST and I'm CST I played around with it for a while and found out that it works as expected only when I create a section of a hole. It must be some ISO standard type of thing I guess. Maybe ISO standards dictate that all holes be shown in a cross section or something? Not sure...guess I'm in for a whole new world of learning about drawings working in an ISO environment.

 

[JohnRBaker]

The real reason that it appears as if the thread is being shown as a solid curve is because you created the threaded holes with the 'Chamfer' option toggled ON which means is that in your drawing what you're seeing are the edges of the Chamfer. And even if the chamfer what not there, the ISO standard does NOT use a dashed curve to indicate a threaded hole but rather a partial arc which, if you stop and think about it, shows more accurately what you would actually see in the physical model.

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.

 

[scottpainter]

Thanks again for the catch on that. Another lovely 'default' set up by parent company...

Riddle me this though, why then does the Feature Parameters method of putting a call out on a hole still not call out the depth unless I switch to ANSI mm when creating the Feature Parameter callout? In order for it to call out the depth I need to create a section.

 

[JohnRBaker]

Prior to NX 9.0 the hole feature drawing call outs are being controlled by a 'template' file where the format of the various hole types are laid-out. Unfortunately each 'standard' has it's own set of templates and these are not available for customer editing and updating. Unfortunately they were developed over a period of time and not always by the same person and things were missed. For NX 9.0 we've implemented a new approached, which will be supported for BOTH traditional Drawing creation and PMI, where you will have direct control, via an interactive 'settings' dislog and customer defaults, of the contents of the call-out annotation and it will include all of the 'features' available when defining the hole feature in the model, including type, depth, clearance/fit, thread size, etc.

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.

 

[scottpainter]

Thanks again for all the help/answers. I appreciate it. I've been told that we can't call GTAC due to the fact that we either bought the software or the licenses in Germany thru our parent company. I can't find anybody who can get me the sold to ID. I am one of two people at this location that use UG and I've been here 4 weeks now. We had someone who had a lot of tribal knowledge, but she was separated from the company about a week and a half after I started. So, I'm sort of on my own here. Thanks again. BTW... you wouldn't happen to have a list of all the companies in the Chicagoland area that use NX would you? I recently relocated back to the area from San Diego and having a hard time finding potential employers...

 

[JohnRBaker]

While we can't disclose our customer lists, if you're located in Chicago you're in luck. Next Tuesday, October 8th, there will be a Chicago/Wisconsin Area Regional Users Meeting in Gurnee, IL. This is one of the larger and better attended RUG (Regional Users Group) meetings and many customer will be there as well as PLM partners and several people from Siemens PLM Software, including myself. There will also be a series of FREE training classes covering several basic topics.

For more information about this Users Meeting, go to:

http://www.plmworld.org/caugwugrugevent

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.

 

[scottpainter]

Somehow I knew you were going to mention that...

I'd love to go to it, especially to meet you after having read your input on here for several years. In a strange twist of irony though, I will be flying out to San Diego that day and can't attend. I'll keep an eye out for the next one out here though. Thanks again for all your help.

 

[JohnRBaker]

Well the next two Regional meetings relatively close to "Chicagoland" will be Detroit on November 5th and West Lafayette, IN (Purdue University) on November 14th.

For information on the Detroit area meeting, go to:

http://www.plmworld.org/detroitrugevent

For the West Lafayette area meeting, go to:

http://www.plmworld.org/indianarugevent

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.

 

[scottpainter]

Thanks for the head's up. The Purdue one might work, but I don't know if it would be attended by as many Chicago companies at the Chicago one. Maybe I'll just send my wife to the Chicago one with a handful of my resumes...

Do you know of many companies in the Chicago area that need people with surfacing experience. My most recent work was in the golf industry and I would like to find something out this way that has the same surfacing challenges I faced while developing golf clubs. I don't expect you to give up names of companies, just wondering if you know if there are any out this way.