Broken view in drafting; NX5

[lurks]

I have a part that is 8' long and need to "cut" it three times to capture everything in the drawing. I am trying to use the broken view tool, but it is only allowing me to "break" it one time. Does anybody know how to do this or understand what I'm trying to do?

Thanks in advance,

Lurks

 

[hudson888]

So what you're saying is that you cannot generate a broken view from another broken view.

I guess that may be the case and that the solution becomes to create curves for the break points and use them in generating a "Break Line/Detail" boundary manually. If you're on NX-5 or lower the technique is usually achieved using expand member view to create the break line curves. You may be familiar enough to forgo a blow by blow account of the workflow, but if not post back.

I believe that expand member view may not exist under NX-6 so I'm interested to hear what the technique would be going forward.

Cheers

Hudson

 

[JohnRBaker]

I just created a broken view, using NX 5, with 3 segments. No problem at all. What you need to do is to continue to define the view boundaries and the anchor points, hitting apply when you're done with each segment, and then while still in the dialog, go to the next segment and continue, repeating the steps until all of the segments are defined and then when you're done, select 'Display Drawing Sheet' and you will have as many segments as needed as a series of 'Broken Views', as in the attached example drawing.

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.

 

[hudson888]

The post doesn't say what release Lurks was using. I think you can maybe do in NX-5 what would not earlier have worked and that could explain the situation.

Best Regards

Hudson

 

[JohnRBaker]

The post doesn't say what release Lurks was using.

He certainly does...look at the title of the thread ;-)

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.

 

[lurks]

How do you define an anchor point? What is considered a good anchor point? I have attached a file of the part that I am working with.

 

[JohnRBaker]

Basically an anchor point should be some point (end point, arc center, etc) which will always be inside the view segment being defined and ideally one that will not move relative to the details which you created the view segment to isolate in the first place. In my example I used the 'arc centers' of the 3 holes. That way, if the hole moves the broken view segment will also move so that the anchor point and all of the model detail near it will still be visible in the broken view segment. In your example I would suspect that the arc centers of the holes would also be ideal 'anchor points'.

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.

 

[lurks]

Thank you, that worked perfectly.

 

[man2007]

I think you can maybe do in NX-5 what would not earlier have worked and that could explain the situation.

You can create it in NX2, NX4 as well.