remove solid object from view 2

[Berserk]

Hello,

UGNX3 Windows XP SP3

How do you remove a solid object from a view?
I have two files, one model, the other the drawing.
The model is composed of hoses and connectors.
If this is an assembly, I could remove one of the components.

Since the model is one file, whenever I try to blank one of the solids, it affects the other views as well.

TIA

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[jerry1423]

No, do not blank it.

If you want to remove it just from that view you can put it on a differnt layer and use "visible in view".

You can also erase just that solid body from the view (located in view dependent edit).
If you do erase it then make sure only "solid body" is toggled on so that it picks the entire body and not just the solid edges.

 

[Berserk]

Hello,

Yes I cannot blank it without affecting the other views.

I would prefer to leave the layers "as is".

When I try to erase using "view dependent edit" and try to select the solid, it won't let me. When the selection filter is set to any, I could select the edges/curves on the view.
If set to solid, I can't select anything.

Model representation is "part" and is fully loaded.
If I go to modelling and try to blank the solid just to test if it is really a solid, it works.

Productive Design Services

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[Berserk]

ooppss!

I got the view set as "extracted edges"
When I removed the check mark, it works now.

Thanks!

Productive Design Services

http://www.productivedesign.com

 

[cowski]

Another method is to use the 'hide component' command. In NX2 this can be found in the Assemblies -> exploded view menu (in NX 6 it is called 'hide component in view' and can be found in the Assemblies -> context control menu). When you run the command it will prompt you to pick a component (you can pick from any view) and then it will prompt for a view. It will then hide the component you select in the view you select.

I will often use this command on assembly drawings where I have an exploded view and an assembled view. I can select all the interior parts from the exploded view and make them hidden in the assembled view. This speeds up subsequent view updates on the assembled view.

 

[BOPdesigner]

I don't think there is an assembly to hide components in. From the problem description, there is one part file with multiple bodies. So I believe visible in view (different layers) or erasing via view dependent edits are the only options.

 

[cowski]

My apologies, I missed the point that the model was all in one file.

Since that is the case, ignore my post - jerry hit it on the head.

 

[hudson888]

If the model is all in one file but the drawing in a separate file you could do something nasty with reference sets loading two copies of the component hiding components in views and excluding the double up from the parts list. Since I abhor reference sets in assemblies I'd walk a country mile to avoid creating such a mess. even though I'm telling you now that it can be done it is only so say that somebody will probably alert you to it eventually and I'd sooner caution against creating a mess in advance.

You would be better to split the single assembly file into two assemblies all things being equal just to make it work better. Then you can hide components in views with little or no trouble.

What I would do is to move one of the solids to another layer in the drawing only. Then I'd set visible in view on the drawing views. The practical advantage of this is that we often wish to create a drawing of a part or assembly that is already released. Our released parts are write locked so you can't alter the layers, reference sets, or assembly structure to suit your drawing requirements. That is why we conform to a standard which uses layers on occasion to maintain the independence of model and drawing requirements. Best practice is always to assign categories to the layers you use and work within a predefined accepted standard.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[ewh]

I would follow cowski's or hudson's advice. Try not to make it more complex than you need to.

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

 

[Berserk]

Thanks for all the reply.
Anyways, here is what I did.

I just use the "view dependent edit" to "erase" the solid object.

The first time I tried this, I can't select the solid object.
This is because when I created the views, I have "extracted edges" checked. I forgot about this. I usually leave this checked so that when someone looks at the drawing file without the model file, they could still see the views.

I can't move the solid objects to different layers because GM wants the solid geometry that defines the part in layer 1.

I would have preferred to have a model file for each solid object (which I think is the proper way) but the file came "as is" from our customer and they do not want us to modify it. Just create the drawing.



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[hudson888]

Just so we're clear on the GM standards I think you should check.

GM want the Solid object that creates the part on layer 1 of the model. You can move the solid body to another layer in the drawing file while leaving it on layer 1 in the model file. For the drawing there is no such applicable standard. And this allows you to set visible in view masks. Either that or your office is interpreting the standards entirely differently to what we have been held to in the past.

I know what you mean about supplier assemblies and I agree to some extent. The problem is that somebody came up with a formula that says it costs so much per part to create a part number and so they simply want to maintain fewer files on their system. The result is that you have things called assemblies that consist of models with multiple solids, and no components. The language gets confusing.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[Berserk]

Yes Hudson, you are right about the GM standards regarding the drawing files. I do not know why I didn't do it that way.

I remember doing it on another program where I have the side marker on a layer and the sheet metal that it attaches too on another so I can control what is visible on a view using layers.

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