How we will create dimensions in angle with X,y and z directions in NX 1

[tonyjosephpaul]

How we will create dimensions in angle with X,y and z directions in NX6?
AS an example,I have to create a dimension with an 10 deg angle.

 

[tonyjosephpaul]

Please refer the attached snaphot.Can we create dimension between A-A parallel to line B-B(10 deg from base) .

 

[PDW]

Hi Tony and a few more,

What version of NX are you working?


Best regards,

Pascal,

NX5.04+TC2007 (GM Toolkit) / NX7.5 native

 

[looslib]

To get the 10 degree angle you have drawn, click the right end of each line, then place the dimension.

That should have been covered in basic training. It is also covered in the online help and the documentation that comes with NX.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[PDW]

Hi Looslib,

Maybe they want to create a Parallel Dimension and having another measurement direction.
This is an enhancement in NX7 or NX7.5 (Not sure which version it applied)?

Grtz,


Best regards,

Pascal,

NX5.04+TC2007 (GM Toolkit) / NX7.5 native

 

[SiW979]

Do you mean like I have detailed in this video?

http://screencast.com/t/p9PtM4TZ3Gyd

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX7.5 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[JohnRBaker]

I suspect that this (see the attached video) is closer to what is being asked for.

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.

 

[SiW979]

That makes more sense John.

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX7.5 native)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[tonyjosephpaul]

Hi John,

The video answers my question.But can we do it in NX6?

Thanks

Tony

 

[JohnRBaker]

In NX 6.0 you'll have to work a bit harder, but it can be done.

In your drawing, 'Expand' the view which you wish to dimension and then under...

Format -> WCS -> Orient...

...set the type to 'X-Axis, Y-Axis' and which the selection scope set to 'Entire Assembly', select the 10 degree 'line' as the X-Axis. You can select anything else for the Y-Axis since only the first selection will determine the orientation. Once the WCS has been redefined, you can now use the normal 'Horizontal' dimension and select the two points of interest. Now unexpand the view and you should be good to go.

It should be obvious now why we enhanced NX 7.5 to allow you do redefine the 'dimension axis' on-the-fly as shown in my video.

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.

 

[tonyjosephpaul]

thanks,John.That answers my question.

Thanks,

Tony Paul
Karayamparambu