NX 8.5 drafting 1

• Feb 8, 2016

• #2

Xwheelguy

Automotive

Mar 17, 2004

2,048

US

For the first issue, if you can include either a 2D or 3D Centerline in that view, you can select it and the dimension should double if you're using a Cylindrical dimension. You may have to enlarge your view boundary and/or make the 2D/3D Centerline view dependent (expand the view then insert 2D/3D Centerline, expand out of the view, create dimension, fix view boundary).

Not sure what your question is with the second issue. Are you trying to change the display of the threads? If so, that may be a part specific setting meaning only new parts will be affected by changing the customer defaults. You'll have to change that via the View Style/Settings dialog. Do not forget for a change in customer defaults to take effect, you must restart NX for it to take effect. If you're using a template, changing the customer defaults won't have an effect on the template file.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

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• Feb 8, 2016

• Thread starter
• #3

aleksandar81

Mechanical

Jul 2, 2014

137

BA

Thank you,my second question is how in section I can dimension thread.I only see this option as hole callout in radial dialog for threads in view.Here is for NX 9,same is for NX8.5.

What I want is this

 

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• Feb 9, 2016

• #4

JohnRBaker

Mechanical

Jun 1, 2006

38,283

US

There's a 'Hole Callout' option available with liner (Horizontal or Vertical) dimensions as well.

John R. Baker, P.E.
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

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• Feb 10, 2016

• Thread starter
• #5

aleksandar81

Mechanical

Jul 2, 2014

137

BA

Thank you John!


@Xwheelguy

Cylindrical dimension can't do this, it gives only dimension value between two points.

 

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• Feb 10, 2016

• #6

ewh

Aerospace

Mar 28, 2003

6,150

US

Cylindrical dimension can't do this, it gives only dimension value between two points

Click to expand...

I beg to differ... it has always worked for me as long as the centerline is picked first and the edge of the cylinder second.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

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• Feb 10, 2016

• Thread starter
• #7

aleksandar81

Mechanical

Jul 2, 2014

137

BA

@ewh


I tried that and it did work, except when the centerline is outside of section boundary.D302,1 is the true diametar.Thank you all very much.

 

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• Feb 10, 2016

• #8

ewh

Aerospace

Mar 28, 2003

6,150

US

There may be other issues involved, as I am able to get true diameter dimensions using a centerline within the same view and the edge as well as using centerlines from other views (as long as it represents the same axis and orientation).

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

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• Feb 10, 2016

• Thread starter
• #9

aleksandar81

Mechanical

Jul 2, 2014

137

BA

I guess, I will have to stick with the centerline within the boundary. There could be the issue with my NX since D296,7 doesn't have any sense.

 

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• Feb 13, 2016

• #10

niedzviedz

Mechanical

Apr 1, 2012

307

PL

First You have to create centerline of hole. Use 3D centerline which will automatic place in center of hole. Then You have to choose cylindrical dimension. Next select centreline and second edge of hole. You should receive something like on Your last picture, first section. Then select this dimension, right click style, go to dimension tab and deselect left | and lest arrow. You should get diameter like on first picture in this thread.

With best regards
Michael

 

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• Feb 15, 2016

• #11

Xwheelguy

Automotive

Mar 17, 2004

2,048

US

The Centerline can be View Dependent if you do not wish to see it. The View Boundary can be set to manual and you can hide it after placing the dimension.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

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• Feb 15, 2016

• Thread starter
• #12

aleksandar81

Mechanical

Jul 2, 2014

137

BA

Thank you guys

 

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• Feb 15, 2016

• #13

Xwheelguy

Automotive

Mar 17, 2004

2,048

US

Here's a video if anyone wants to see what I mean by making the Centerline View Dependent and adjusting the View Boundary.

centerline.zip

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

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• Feb 16, 2016

• #14

kevinmcc

Aerospace

Jul 12, 2010

2

US

Or you can just create and name the centerline in modeling under properties
and then you can reference it in drafting as your first pick without
going in and out of view dependent edit.

 

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• Feb 17, 2016

• Thread starter
• #15

aleksandar81

Mechanical

Jul 2, 2014

137

BA

How can you create centerline under properties?

 

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• Feb 18, 2016

1
• #16

kevinmcc

Aerospace

Jul 12, 2010

2

US

Here's a word document on how to dimension using a named centerline.
This is for NX8.5 and earlier. From NX9 and beyond it's a totally
different process using a "name selection" box and a few other different things of course.

 

 http://files.engineering.com/getfile.aspx?folder=f1c48590-e7a9-4058-9997-bd596f6137b3&file=diameter_dimensioning.docx

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