My assembly shows up as "Part is Reference Only" in drawing

[danicole]

I am using UG NX 7.5. I am relatively new to this software (usually use Pro/E) but our customer is requiring a native UG drawing. I created the assembly in modeling with constraints and opened a drawing template to place the views but the assembly shows up as a Reference part in the Assembly navigator (under the Info column) and when I go to modeling view display (under Display Sheet), the assembly model doesn't show up (empty with just the coordinate system).

Another thing I cannot get to work is getting a x,y,z coordinate grid in the drawing without having to create physical datums in modeling mode.

Any help would be appreciated. Thanks.

 

[SiW979]

If you right click on the part in the Assembly Navigator and click properties, then there will be a button you can toggle on or off for component is reference only.

cheers

Si

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[cowski]

Not sure if this is the type of grid you are looking for, but while in drafting go to Preferences -> Grid and work plane... This will allow you to specify and show a 2D grid of points that you can use for reference or optionally snap objects to.

www.nxjournaling.com

 

[danicole]

JCBCAD- I do not see a toggle button under properties. I see 6 tabs when I open properties: Assembly, General, Attributes, Parameters, Weight and Part File. I do not see anything regarding component is refernce only under any of these tabs.

Under the Attributes tab it has 3 columns: Title, Value and Type. There are 3 rows with the following names: PLIST_IGNORE_MEMBER, PLIST_IGNORE_SUBASSEMBLY and REFERENCE_COMPONENT. All these have a "String" type assigned. I have tried to highlight & change the Type or even delete and it will not let me.

COWSKI- Yeah, that's not really what I was looking for. I need a line grid that is defined within the borders of the drawing views that corresponds to the offset distances of the Absolute datum planes x,y,z. All our measurements are taken from in-car position and there is a point chart on the drawing that should coorespond to the the coordinate grid in the views. For example, the first vertical line would represent an offset of 2200mm in the positive x direction, labeled X2200. The next one would be offset 100mm from that and labeled X2300 and so on.

 

[SiW979]

OK, so you are not running Teamcenter, but it's the PLIST_IGNORE_MEMBER that is causing your part to display as reference only. I'm not sure how to delete this.

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[matnas]

Hove do you create the drawing

A:
- File -> New
- Drawing tab
- Select template (reference existing)
- Select your assembly under "Part to create a drawing of"
- Add views

B:

- Open drawing template
- Base view-> select your assembly in part section of the command.
- Create views

C:

- Open drawing template
- Add your assembly with add component command
- Base view -> elect your assembly in part section of the command.
- Creat views

If you use A or C you won't get part is reference only

I think B was added for migrating I-deas drawing because in I-deas you could add views from many parts/assemblies to the same drawing.

Style-> General tab on the view if Reference is checked you won't see anything in the view.

Mattias


NX5, NX6, NX7.5 and NX8
I-deas 12, NX I-deas6.1m1
Solid Works 2009 and 2012

 

[danicole]

I was doing option B. So I just tried saving the template in the UG templates folder on my C: drive but it's not showing up when I go to File New Drawing. Is there a specific naming format that I need in order to make it show up in the templates library?

 

[matnas]

you must edit ugs_drawing_templates.pax in the same folder

Mattias

NX5, NX6, NX7.5 and NX8
I-deas 12, NX I-deas6.1m1
Solid Works 2009 and 2012

 

[danicole]

Can you provide more information on how to edit that file?

 

[cubalibre000]

The reason is you have set this option

http://www.eng-tips.com/viewthread.cfm?qid=329050

in the customer default.

Thank you...

Using NX 8 and TC9.1

 

[Toost]

Here's how to edit the .pax file using notepad.
First make a copy of the paxfile, then edit the original. If enter "typos", the drawing tab will not show up at all in the File new dialog.
See image.

Regards,
Tomas

 

[BOPdesigner]

So if we have this case in NX 7.5 (native). Is it possible to replace the reference view part in the ANT with the same part as a component in the ANT so that you can see it in the Modeling application of the drawing assembly.