NX5 - how do you lay down dimensions on an iso view? 1

[RobLN]

I have a 3D exploded view (NX5 Drafting) and I would like to add my dimensions in the same iso orientation as the exploded geometry. Is this possible in NX5?

NB. I'm not sure what the license deal is regarding the PMI I don't seem to have any options to 'add dimension' in the 3D environment but I can put in Notes, Symbols & security marking...

There is a pic attached below to illustrate what I mean...

Any advice greatly appreciated...

R.

 

[hudson888]

Sorry but if you're already showing me that how did you do it?
What are we in fact looking at here.

You can do something like that in NX by working inside the expanded view from drafting, or adding all the dimensions in the modelling environment before you add the view to the drawing. You will have a few issues with the scale of the dimensions and text being subject to the scale of the view, and you will need to orient your WCS carefully before placing some of the dimensions.

There is more than one way to do it but probably none that are really intended to be used thus.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[RobLN]

Hi Hudson

I-Deas is very good for PMI It's actually drawn in I-Deas V12.

Now I need to do the same thing in NX5 - looks like Siemens wants some more money for that PMI bit. I'm checking with the administration to see what we've paid for.

Is there a way of adding in dimensions in that way without a full PMI add on?

Best regards - Rob

 

[ewh]

Yes. In modeling, enter the drafting application. Cancel before defining your drawing sheet so that you remain in model space. You can now apply dimensions, but they will be dependent on the WCS (more so than they would in PMI).

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[JohnRBaker]

Yes there is. Go ahead and create your drawing and place your auxiliary view in the orientation you wish. This can be done by either creating and saving a properly oriented view while still in modeling and then add that view to your drawing, or you can use the 'Orient View' tool when adding the view to the drawing and just rotate it around until you get your desired orientation and then just place the view.

Once the view is on your drawing, select it and press MB3 and select the Expand Member View option. Once the view is expanded you should turn on the display of the WCS and then orient it so that the X (horizontal) and Y (vertical) axis align with face from which you wish to select edges to dimension such as seen in your example image. Note that you will need to move the WCS each time you wish to change the X (horizontal) and Y (vertical) axis orientation of your dimensions. Once all of the your dimensions have been placed, again select the boarder of the view, press MB3 and toggle OFF the Expand Member View option. And this should do it.

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.

 

[RobLN]

Hi John

Thanks very much that is exactly what I wanted, and way easier than I expected it to be as well.

Best regards Rob.