SIMPLE way of controlling drawing view display

[Ritchie]

Hello NX users,

Just a very simple question, to which I hope there is a very simple answer.

I'm making a drawing of a 3D assembly (by means of the master model method) but I find it extremely annoying and complicated to control the way the 2D drawing is being displayed.

Some components of the assembly have WAVE linked geometry in them. In the 3D assembly display this geometry is hidden, yet it shows up on the 2D drawing view of this assembly. So in other words the 2D display does not correspond to the 3D display, which is rather annoying.

It would be very satisfying if I can get NX (8.5) to simply display the drawing view the way as it is displayed in 3D, so without any unwanted surprises of showing hidden geometry. I have gone through the over-elaborate view style menu of the drawing view but a simple toggle to control the drawing view that I'm looking for does not appear to be there. Surely I'm not asking too much and there must be a way to achieve this???

Thanks in advance, sorry for the negative vibe but I'm really annoyed if someting that should be easy con not be achieved in one or two clicks...

 

[ewh]

Have you investigated the Visible-In-View settings in your model and drawing?

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[Ritchie]

No, should I? If so, where can I find them?

 

[cowski]

Reference sets are used to filter what you see in the assembly (and the corresponding drawing view).

www.nxjournaling.com

 

[ewh]

But he is seeing different solids in the model than he is in the drawing.

Ritchie,
In NX6, Visible-In-View is found under the Format tab. In the drawing, find out which layers are visible in the views. That will tell you what layers you are and aren't seeing in the drawing. Make all layers selectable, go into the model, open up a canned view and go to Format -> Visible In View, Reset to Global, Cancel. Then Show All (in case something had been hidden).
Now you should be able to see most everything in the model. From there you should be able to sort out why the drawing/model appear as they do.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[Xwheelguy]

Let's add another route to make it even more confusing....

Hide Components In View.

In Drafting, select Assemblies -> Context Control -> Hide Components In View. Next, select the components you do not wish to see (from either the ANT or dwg views), then select the view(s) in which you do not wish to see them. Update the view(s). Done.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[ewh]

But his hidden components are in modeling, not drafting (if I am understanding correctly).

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[Ritchie]

True, they are hidden in modelling and shown in drafting.

Man this is complicated. So both layers and reference sets influence the way the model is displayed? I have not worked with any of these features, so I guess I have always used the default settings. Meaning no predefined reference set and everything on the same layer.

Is there really no simple way to display the model "as it is in 3D" in a 2D drawing?

Thanks for the help so far!

 

[cowski]

Reference sets are used to filter what you see in the assembly (and the corresponding drawing view).

But he is seeing different solids in the model than he is in the drawing.

Let me clarify:
I wasn't trying to diagnose why different entities are seen in the model vs the drawing. I was offering a solution to filter out unwanted geometry in the model so that the drawing will match. Assuming the master model method is being used, reference sets are a good way to do this.

www.nxjournaling.com

 

[NutAce]

Hello Ritchie.

The reason why you see your wave linked geometry in your drawing is because it is probably in the reference set you are showing on your drawing.
By default this will be ref set "model".

For each component which has wave linked bodies in your assembly you need to state what the reference set needs to show.
If you go into the reference set menu. (Format - reference sets) and you select the referense set "model" you can select which geometry needs to be in that reference set.
By default all 3D geometry will be in there which includes the wave linked geometry. (through the customer defaults it can be arranged to not automatically add wave linked geometry)
Now if you dont want to see the wave linked geometry you just remove it from the reference set. ( you first need to unhide the geometry to be able to deselect it).
I always find it easiest to first deselect all geometry and then add the things I do want to be in there...

Reference sets reflect on the toplevel of your assembly where your component is used. So now you need to state which reference set is to be used for your component in your working assembly.
You can do this by right clicking on the component (assembly navigator) and then select "replace reference set" By default it will be on reference set "model" so you probably don't have to change it.

Now because you are working master model, your drawing will be the Parent of your assembly. So your 3D assembly will show as a child for which you can change the reference set.
Make sure that the reference set selected is "Model". On the drawing you should only see the geometry which is in there.

Keep in mind that reference sets will reflect only one level up in an assembly so for each sub-assembly you need to arrange this seperatly.



Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.2 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

 

[Ritchie]

Great answers, thanks for the replies! My NX is an out of the box installation so I guess it needs some tweaking.

 

[ewh]

The reason why you see your wave linked geometry in your drawing is because it is probably in the reference set you are showing on your drawing.

But why isn't the geometry showing in the model?

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[NutAce]

But why isn't the geometry showing in the model?

Probably because when creating the wave link the option "Hide original" was set.
But this is not preventing it from being added to the reference set. And if that reference set is selected for the drawing it will still show.

All 3D geometry you create in a part will be automatically added to the reference set model. (OOTB)
This will go for wave linked created geometry as well. (unless otherwise set in customer defaults).



Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.2 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

 

[ewh]

Yes, but such geometry usually appears in the model.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV