Hiding bodies in drawing

[rossob]

I'm just wondering if there is a way you can hide certain bodies of a component in a drawing? We have an item which is essentially a piece of angle with a 5mm end cap (see attached image). This item is purchased as a single item, with only one part number. The current drawing (done in Mechanical Desktop quite some time ago) has localised parts and the drawing shows the fabrication details of the complete item, but also a detail view of ONLY the end cap.

I have modelled this in NX using two extrudes, and thought that if I created a drawing I could just show a detail of the end cap, somehow, by just hiding the piece of angle. I can't seem to be able to make this work. Is there a way i can do this, without making this item an assembly of two parts?

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[JohnRBaker]

Create a Reference Set which contains only the solid body that you wish to see in your drawing. Then when you create your master model drawing, set the Component to the Reference Set that you defined.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Either that or push what you don't want to see to a different layer in the drawing file again using master model concept. That way you can more easily set visible in view to enable the display of only certain objects.

Now the reason I mention this one and that it gets used more often than not, is that you may find that you don't own the model file. If that is the case then you can't always make the reference set solution stick.

Regards

Hudson

 

[rossob]

I did try the reference set approach, but I found that the reference set controlled the whole drawing, and not just the view I want to change.

We are trying to steer away from using layers (except for drawing borders)if possible, just using show/hide for datums/reference sketches, etc.

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[JohnRBaker]

You have to use Master Model to make Reference Sets work the way they were designed to work. If people don't use master model we can't be expected to create another solution to a problem that we have already solved.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Ross,

I think you might be up against one of those if possible situations where you need to use layers. I can't see why you'd want to avoid using layers, but unless some better solution can be found for you I would suppose you're better off making an exception at least for this case.

Good luck

Hudson

 

[4mranch1]

With the drawing open select a face on the the component you wish to hide / MB3 / Show-Hide / Hide Component

This will Hide the component in that particular view only.

Gary Ashby
Designer

 

[4mranch1]

Disregard the previous post I thought I was in the SolidWorks forum.

In UG/NX3, and later, another way to blank/hide a component in a view is as follows:

Select View / MB3 / View Dependent Edit... / Erase Objects / Class Selection / Type / Solid Body / Select body you want to blank/hide / OK / OK / OK / Update view

Gary Ashby
Designer

 

[ewh]

If using layers is off of the board, I would go with Gary's suggestion.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[hudson888]

My understanding was that it is not a component that needs to be hidden. Rather instead it is one solid body of several in a component.

Regards

Hudson

 

[ewh]

...which is why you can't hide the component in the view, but you can erase a solid body without affecting the rest of that component.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[vitulin]

I have a question. It is possible to set the layers shown on a drawing view. Is it also possible to have different reference sets on drawing views?

Thanks
Vit

 

[rossob]

John, sorry about the misunderstanding. I didn't realise there were so many different ways to create drawings which all give different results. I have just undertaken our essentials training, and have intermediate next week, but not done the drafting side yet.

I did try the master model approach and found that I could add another view, and then change the reference set of that view to hide/show the component I didn't want to see. I did find, however, that if i were then to add another view to the drawing, that view was tied to the selected reference set and couldn't be changed. This could be a pain, if

I also was able to hide solid bodies(using Gary's suggestion)which worked fine.

I think, to maintain full functionality and control over these items, maybe best for us to stick to assembling parts, instead of single parts made of solid bodies.

Thanks again guys. I have found this forum to be a great source of information. Keep up the great work

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[hudson888]

No I don't believe that it is. You can only have one reference set per component at any given time. You could theoretically have the component loaded twice each with a different reference set and then go about hiding the double up that you don't want in every other view. You could but I'd probably have to kill you for that if I was the next guy using your file.

I take into account that you don't know that in all cases you will have write access to change a the component that you're adding, meaning that if you can't save the file that is added to your drawing in master model concept then you can't effectively add the extra reference set. Therefore I have to say that layers are the tool of choice because you can get this to work as a filter using visible in view in all cases under pretty much any circumstances.

There has been some discussion on the forum about the use of layers and other methods of hiding or showing geometry, view dependent or what not. There are a lot of methods perhaps too many that really represent legacy techniques that tend to overlap too much, so that you can find yourself with objects in the file that are unnecessary difficult to find. And while I hate that and shun some methods I am perplexed that layers have become unpopular with some as I find them reasonably easy and straightforward to use. Somebody tell me what the problems are that you have with layers. If I'm wrong change my mind for me by all means.

Otherwise there is a technique called defining reference sets in views, which changes the line type or font so that some components can use hidden line removal and others are shown in phantom outline. It supports a method of showing reference components especially used in tooling drawings that has wide historical usage as a standard drafting practice that some may be familiar with. It has never supported making the line font invisible in the same way that is possible using view dependent edits. Neither of these do what you want, and nor are they currently intended for that purpose. In view dependently erasing all or part of an object don't expect the capacity to restore what is hidden behind. However defined render sets can kind of mirror reference sets in the scope of what can be selected, and the Hidden Line and Phantom Visible line combinations currently provide the capacity to reveal solids hidden by other solids. Perhaps it will in future versions be possible to make visible lines of selected solids invisible using defined reference sets. Although it may sound anachronistic perhaps it is one way we could get around these kinds of problems without using layers. Whether in providing this you create yet another kind of filter that hides things where nobody can find them or work out how you did it is altogether another question. Maybe I'd rather stick with the solution I know.

So I'm hearing that layers are on the out, but in thinking what is or could be available to replace their functions I wonder if we would be better off.

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

What I believe Ross stumbled across was the ability to add a view of a part, meaning of a part OTHER than the one that the drawing is of, except that of course there is nothing stopping you from picking the same part a second time. Are we all throughly confused yet?

Anyway, this just might be the better approach since it will allow you to add at least one more view which can use a different Reference Set since in essence, when working in Master Model, the component has in fact been added twice, but unlike what happens if you just did by just adding another component as such, is that it has it's own graphics space (you never see both parts in the same view) and the second component never gets included in the Parts List, which is also important because you didn't really add it because you wanted two of them, just because you wanted to SEE IT TWICE, just slightly different in the second view.

Not to really confuse you all, but if this had been a drawing of a true assembly (a part with multiple components itself) and you wanted a second view with different content or parts in a different position, like two view of a butterfly valve, open view showing the valve open and the other showing it closed, you would still use this View From a Part, just that rather than changing Reference Sets, you would use Assembly Arrangements, another scheme developed specifically for Assemblies to control the content and positioning of components of as assembly so that you can show DIFFERENT 'arrangements' of the same assembly. This was done in part so that users did NOT have to resort to Reference Sets in an ASSEMBLY which we highly recommend that you NEVER do.

Anyway, I've probably confused the new users enough and so my work is done ;-)


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[rossob]

John, that is exactly what i was trying to say. Just not described as well as you just did. I'm still trying to get up to speed with the terminology for NX.

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[hudson888]

So how do you do it. Do you open the other part create a drawing view, and then copy and paste that to the other drawing in the other file?

We have used exploded views a lot for different positions of components in views within a single drawing, i.e. the famous butterfly valve open and shut scenario.

I hadn't considered or checked out using arrangements to support drawing views I always thought that you could only see one arrangement at a time, and why not since you already have exploded views which seem to do something equivalent. If you can do it then how roughly does it work.

In combination with other problems that we had getting really huge assemblies, i.e. entire vehicles or the body in white to ever produce a hidden line view we often used View>Visualization>Assembly Hidden Line. This makes what is essentially a dead data snapshot of the view. You could use something like that to show different things if you're really only looking for an illustration that doesn't need to be very maintainable. My question would be... Is Ross' accidental technique any more maintainable. Also what if you don't have write access to the component that you're making a drawing of?

So I'd like to have a crack at it myself, does it work in NX-3 or NX-4, or only NX-5? And again roughly how did you achieve this feat?

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

It's true that you can only see one arrangement at a time unless you use the View from a Part option to in essence add a second version of the part in it's own set of views.

As to how you add this different type of view (which we've supported for several releases now) up through NX 4 this view had it's own icon, titled 'Part View' on the Drawing Layout toolbar right next to the 'Base View' icon (which is why we changed how you get to in NX 5). If you select the 'Base View' icon you're adding a view of the part that the drawing is referencing, however, if you select the 'Part View' icon you can select ANY part file you wish to 'added' to the Master Model drawing as a sort of 'reference' view, INCLUDING selecting the same part over again that you are already creating a drawing of. And as I've stated before, this part will have its own graphics space so that it will ONLY appear in the views that you create from what will behave like just another Base View, except that it will NOT be added to the Parts List and it will not be seen if you were to close the drawing (you'll still seen only the original master part). Hence a 'View from another part'.

You can also get to this function from Insert -> View -> Add View from Part...

Now in NX 5, because too many people were confusing this with the regular base view (I mean the icons were right next to each other and they looked virtually the same and ...) we decided to take a different approach. We just have a single 'Base View' icon (and just a 'Base View' option on the Insert -> View pull-down as well) and so we now KNOW that everyone will be going to correct spot and under normal conditions you'll just do what you are being asked to do. However, if you DO wish to add one of these special views, when the 'base View' dialog comes up, at the far left end of the dialog there is an option labeled 'Part' where you can go and optionally select a different part file, or the same one if that's what you want.

What this will also allow you do is support organizations that do not use mono-detail. That is you can make a drawing of an assembly and then using the 'Part View' option, set up base and projected views for each individual detail part that makes up the assembly spread across several sheets if needed yet still all documented on the same 'drawing', and all without messing up the Parts List.

Anyway, I hope that helps explain it all, confusing though it may appear at first, it is a very power capability to have in your back-pocket if you ever need it.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[rossob]

I work for a crane manufacturer and my goal is to be able to produce a load chart drawing with different configurations of the crane. eg boom raised at different angles.

We have figured out that we can do this using arrangements, and have managed to overlay a second drawing view of the crane in a different arrangment over the original view. We have found though, that we are limited to only these two arrangements, while our current load chart has 7 configurations.

Is there something i am doing wrong here John?

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[rossob]

Actually, scratch that, got it working fine.

Have managed to get 4 views overlaying each other. I found that I had to re-browse to that file each time instead of accepting the default drawing view, and then all the different arrangements were able to be selected. I found if i didn't re-browse that file again, I was only able to select from the arrangements that were already placed on the drawing.

Hudson, you will notice in the base view dialogue box there is a button to the right of the scale button where you can choose an arrangment.

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007