Changing Datum in Modelling 1

[Mitchel123]

Hi Guys,

It is going to be a basic question but I never done this before and finding it pretty difficult.

Please see the attached model.The model is created using NX 8

I would like to change the datum of the model so that the holes are in vertical position and when I select the 'Top' option from orientation menu the model should display both holes in vertical position.

This will help me orientate the model correctly in drafting.

Appreciate for your time guys.

Thanks

Mitchel

 

[JohnRBaker]

OK, open your part, go to...

Edit -> Move Object...

...in the 'Transform' section of the dialog, set 'Motion' to 'Align Axis to Vector'. For the 'Specify From Vector' use the 'Two Points' method and select the arc centers of the two holes. Now for the 'Specify Vector' step select the 'Y' axis of the Coordinate system. In the 'Results' section of the dialog make sure that you've selected the 'Move Original' option and then in the 'Settings' section only toggle ON the 'Move Parents' option. Now go back and select the solid body and hit OK. You should be good to go.

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.

 

[cowski]

If your goal is just to orient the part for convenient drafting views, there are other options as well.
[ul][li]If you use the master model drawing method, you can reorient your component in the drawing file. This allows you to pick a convenient orientation for modeling and a different orientation for drafting. In other words, the drafting 'top' view will be different from the modeling 'top' view.[/li]
[li]Orient the view to show what you want as the top view and save the view. You can then generate a 'view set' from this custom top view.[/li][/ul]

The first option changes the orientation of the component, the second option changes the orientation of the 'camera'.

www.nxjournaling.com

 

[SvenBom]

And if you still (for whatever reason) want to place the whole body on a different datum plane, do this:
1. click on the sketch with right mouse button and select Edit with Rollback
2. when you are in sketch environment, click on the Reattach icon. In default installation, you will find in near the 'sketch name' field. Or, you can go into Tools menu. There, it will be near the bottom of the menu.
3. now, select a different datum plane: x-y for example
4. the sketch will be moved to a new plane. When I did this, only one dimension (p2)failed.

But have in mind, that with more complicated models, you will have bigger problems, when using Reattach command. So in many cases, it would be better to do, what John and cowski have already described.

And one more option for drafting.
When you are creating a fist view, you have Orient Tool option (Base View command: section Model View or View Creation Wizard: Orientation Step). With this option, you can orient your model to whatever view you want. Regardless of any top view definition from the model.

Regards.

 

[Mitchel123]

Thank you for your reply guys.

John, Using the option 'Align axis to vector' it all goes well when selecting the the arc centres of the 2 holes and also for its fine with 'Specify Vector' and selecting the 'Y' axis of the Coordinate system. When selecting the body gives an error that 'two axes do not intersect cannot define transformation' Is there anything I am doing wrong?

Thanks

 

[JohnRBaker]

The two 'vectors' have to lie in the same plane, so pick the two arc centers on the same side of your model as where the Sketch is located, as that's also the X-Y plane of the Datum CSYS.

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.