NX11 and Drawing curves not showing in View 1

[isnemo]

Hello,
Here's my scenario:

I have an insert modeled up.
I use drawing templates to create setup sheets.
Drag my template onto my model and it creates the drawings. Now the insert model is a child part of the drawing.
With my drawing part file set as the work and displayed part, and, while in modeling, I save a CSYS.
Go back into drafting and look at my views and the CSYS will not show up.

I've looked to make sure all the appropriate layers are on and visible, check to make sure it wasn't a 'reference set' thing but still no sign of the CSYS in my drawing views. I even tried creating curves (a simple box around the insert) and those curves won't show up either.

Any clue givers out there??
Nemo

 

[joycejo]

When you say "I've looked to make sure all the appropriate layers are on and visible" did you check Layer- Visible in view settings for the drawing views?
This is different than just layer settings. You can have layers visible but if they are not "Visible in view" nothing shows up. This often happens when trying to add geometry on other layers when a view already exists.


John Joyce
Manufacturing Engineer
Senior Aerospace CT
NX 10 & 11.0.1 Vericut 8.0.3

If I asked people what they wanted, they would have said faster horses

- Henry Ford

 

[SDETERS]

Is the drawing view made from the Specification or is made from the actual model?

 

[isnemo]

John,
Yes... kind of what I meant my checking the layer settings. The layer that the curves are on are visible in view as well.

Sdeters...the drawing views are made from the model. However the curves are a member of the parent node (the drawing file itself)
In NX 7.5 any curves I placed in 3D space (with the drawing files as the work and displayed part) I could get to show up in the 2D views simply by putting them on a layer and making it visible in the view.
As you can see in the images the CSYS and curves in my 3D-space IN the dwg.prt file show up in my views in NX7.5 Not so in NX11
Greg
NX7.5

NX11

 

[JohnRBaker]

If you're creating curves in a Drawing view they could be 'view-dependent'. And if you're creating curves in a Part which is a Component in your Drawing 'assy', make sure they have been included in the Reference Set used when creating your Drawing 'assy'.

John R. Baker, P.E. (ret)
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

 

[Xwheelguy]

For clarity, are you using the Master Model method? If so, when you create a drawing base view, NX now asks which of the loaded parts you wish to create a drawing. If you select the component, then you will NEVER see anything you do on the modeling side of the drafting file. I don't think NX did this in NX7.5 (or maybe prior). I do recall it changed at some point and when it did, it took me a bit to get used to it.

For example, let's say your insert is named INSERT.prt and you add that as a component to another file named INSERT_DWG.prt. When you have INSERT_DWG.prt set as the Work Part, create a drawing sheet and then proceed to place the first view using Insert Base View, NX will prompt if you wish to have your views reference INSERT.prt or INSERT_DWG.prt. Most of the time, it is preferred to choose INSERT_DWG.prt as the NX file to reference on the drawing. If you choose INSERT.prt, then whatever entities you create in INSERT_DWG.prt will never show up because you're putting them in the wrong .prt file. See if you draw the box around the insert in the model only file and add them to the appropriate reference set that they then show up on your drawing.

The bad thing is that I don't believe there is an easy fix to correct this - you will have to either remove all your views and add a new base view or just delete the sheet and start all over.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.3
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[jerry1423]

Sometimes when something is not an actual solid body the part must be fully loaded (not just partially) for it to show up properly.

Jerry J.
UGV5-NX11