We are using NX5 which will allow the Type Filter to be changed when the selection menu opens.
Select view > MB# > View Dependent View > Erase Objects > Type Filter > Solid Body > OK > Select solid body in view > OK > Cancel > Update view
In our previous version NX3 you would do the same with View Dependent Edit > Erase Objects > Class Selection > Type > Solid Body > OK > Select solid in view > OK > OK. Then update the view.
PLEASE, DON'T START USING VIEW-DEPENDENT EDIT TO "ERASE" COMPONENTS IN A DRAWING!!!!!!!
While in the drawing, go to Assemblies -> Exploded Views -> Hide Component.
Note that starting in NX 5 we've moved this function to a more logical and easier to find location (the Remove and Restore Component items now have their own icons on the Drafting Edit toolbar).
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
Thanks John, I did not know about this function. I am now a convert and will stop passing along less desireable techniques.
I had seen this function while maipulating and creating exploded views, but thought it only applied to exploded views. It worked for me in NX3 and in its new location in NX5 (Assemblies > Context Control > Hide/Show Component In View...)
I guess PLMS are working on putting this function in an easier to find place for you in the future. I agree there are a few different ways that you can show/hide things in views, View dependent edit, Render Sets, and Hide components all started out with different specific uses, not to mention visible in view with layers etc... I think some could do with rationalizing in terms of where they live in the menu structure. Perhaps until PLMS do more of that for you then you may want to customize your menus so that they all appear together somewhere.
To do it is one particular view you hide a component in an exploded view that you create outside of drafting usually saving a named view in the process. You then add that view to your drawing, then it and views taken from it will have the particular component hidden in them.
If you have already created the views and want to hide a component you're out of luck. The work around, (which some people don't like to do), is to move the component that you don't want to see to an empty layer, then set visible in view in the the drafting views so that you can see it in some views and not others. This works according to whether the layer is visible in each view then you can only see what components are on the visible layers. If you haven't used this before the hidden line display and all other aspects of drafting work just fine, and new views thrown off will be created by inheriting the visible in view setting of the parent view.
Putting things on layers was used here in the past, and let me tell you, in the end it will make a mess of things.
I suggest doing as John says I find it the easiest once you get use to it and if something in your model gets moved to a different layer you won't have a mess to figure out later.
Plus we try to have all solids on layer 1 so moving things to other layers is not an option anymore.
I guess it is just a matter of what you're used to. We have models with literally hundreds maybe thousands of features and entities used to create the geometry. The idea that you'd put all that on one layer and call the model maintainable is anathema to some. I think you need to broaden your perspective to be a little more inclusive of others' needs.
In this case imagine that the user has created all the views and done quite a bit of work on the drawing that he does not wish to repeat. I had thought that you may not be able to apply "remove component from view" after you added the view to the drawing. Fortunately this was not the case when I tested it again in NX-4 and NX-5. So you won't be forced by compromise to use layers on this occasion as it turns out.
I'm sorry I guess I wasn't clear. We us all solids on layer 1 and datums on a set of layers and sketches on another set and so on. But all the solids are put on layer 1. This will keep order as long as it is followed.
I guess you still wanted to know how to, after we went off on that tangent there.
NX-4
Assemblies>Exploded Views>Hide Component, then follow the prompts to select the components and then select the view. The selection allows for multiple components but only one view.
NX-5
You can customize this on to different toolbars as well.
In the drafting application, Edit>View>Hide Component in View. Same deal as before follow the prompts to select component/s and then still only one view at a time.
Back to the tangential topic of Layers. Some seem to want to get rid of them, so I'm glad to see your later post, which is pretty much what we do at the moment. Vit was in luck after all and I have posted above to support that.
To the forum in general,
We had a post here the other day about what to do if you have a component comprised of several solids only one of which needed to be hidden, but only in one of several views. Hiding the component wouldn't work, nor would blanking. You could create reference sets and add a second component as a view from another part so it doesn't trouble the parts list, but what if you don't own the other component for write access. Even when it seemed to me that it was obvious that there was an easy solution which would be to put that other solid on a separate layer and use the visible in view. I still got pretty much howled down against using layers.
What is it with layers that is so bad after all this time?
Is there some form of indoctrination going on against layers that I'm largely unaware of outside of what I see here in the forum?
In the usual way of making drawings under the master model concept there is only the border or pattern, notes and dimensions on the face of the drawing and the components added to the file and that is it. Most of the time you can do the whole thing on one layer, though many use a separate layer for the borders. How hard can it be on the odd occasion when you need to that you should put something on an empty layer and label the category for all to find. You can even list the layers in the model navigator for added visibility.
There should be ample freedom from site to site to develop standards that can be understood within the organizational culture. It means that you can develop an expectation about how each other will format their data. But to extend that approach to exclude any tool that others are capable of using, but you're not familiar with, is to adopt a fragile approach to doing things. I see it prompting an ignorance of what can be done so that good tools are often forsaken and the whole system has to be dumbed down to the lowest common denominator.
I don't know about others out there but I see this happening and the anti layer movement has that flavor. In any case I didn't buy an expensive high end CAD system only to have people tell me that it doesn't suit their dumbing down agenda to use all the tools that are available. I say this because right off the bat I may have to work with all of you eventually at some time in the future, and I do wish that that future will be a bright one and not dumbed down.
I'm not sure what is behind the 'layer hate', but in the spirit of internet forums I'll venture an opinion. My guess is either the person that set up the CAD rules learned on a different CAD system or the whole company recently switched from a different CAD program. Thus these people try to use the same paradigms in NX that worked in 'program Z'. There are programs that don't use layers, some let you create a (theoretically) unlimited number of layers. Likewise I think some people use the sketcher when there is really no good reason to, simply because 'program Y' trained them to use a sketch any time they wanted to create lines/curves/points.
If this post describes you, please be open about learning what NX can/can't do, it will be easier than trying to force NX to be what it is not. If you are just 'following the rules', you may want to kindly question why the rule exists. Sometimes there will be a good reason, many times you will get a response (like I have) to the effect of - "We tried that feature when it was introduced in version 14 and it was buggy so we don't ever use it" (I was surprised that no one thought it may have been improved in the subsequent versions).
I thought I was going quietly mad. I see as many closed minds against sketcher among some of my colleagues as I see against layers on occasion when I post here. Frankly I know that I'm not learning as much from my colleagues as I have from opening my mind to what I have been learning by posting on the forum. Most people wouldn't realize that many who can help with answers probably go and perform a little test to check or even expand their knowledge before they commit an answer to writing. In this recent case with Vit I learned something about a better approach than what I had thought was technically possible, and now I have a new tool in my kit to take away from the experience.
I think you're right about the users coming from other CAD systems. I have done the same in reverse myself and know that you try to exchange one set of jargon for another and apply the strategies that you know from experience. Also I've posted in the past about the importance of understanding the difference between training and experience being that experience enables you to that the techniques you were taught and develop them into strategies for tackling real life problems.
All that said and while I find an understanding of where others are at and what they bring to a discussion helpful to me, I am nonetheless encouraged when I hear from you because I think it is incumbent upon the experienced users to either enlighten others or accept that in many places the way they use NX will just get dumbed down.
And yes the older hands are still learning too. It just wouldn't hold out interest otherwise. The last paragraph that Cowski wrote is spot on. It strikes a balance between learning and ignorance while encouraging open minds on both sides. I would only add that NX is a tool it has to be designed to be used for its intended purpose. You can use a good tool badly as surely as you can use a bad tool well, so by all means lets try to get the most we can out of it.
I'm thinking you are receiving a wrong message about layers here. I do not hate layers what I hate is no guide lines that are followed. Most of our designs are quite complex and go through many changes and a lot of users. There are so many ways to do the same job in NX none are completely wrong but when a user opens a file and knows what layer he needs to address to make the changes he needs to it goes a lot quicker and smoother.
Another thing I've seen with layers is to designate a layer a "junk" layer where they park all the stuff not needed in a file. If its junk get rid of it some of our files and assemblies are so large we were forced into switching to 64 bit platforms with 12 gig of ram.
Anyway what I am saying is you are much better off getting your users together and setting up some layer rules it will payoff in the long run.
NX-5 makes some steps in what may be for some a helpful direction with their part templates. Even straight out of the box there are some supplied templates with designated layers for common file structures. If your company doesn't use any part templates already perhaps consider adopting something like the standard ones.
Also when you run with master model concept, representations and partial loading in place you don't fill your memory with those construction and junk entities in the files.
By means of occasional incidents that I have observed and experimented to confirm one could argue that you make a considerable reduction in the size of your files by removing all the parameters, and not only because you can delete all the construction geometry. Of course you wouldn't do this and nor-does it directly translate to improved system performance, (where the measures above are in place you may have pretty much equivalent performance). Which simply proves that there has to be room for a common sense application of the tools at hand to come up with an effective solution.
I would say that if all your models are very simple then you may say why maintain a layer standard if you'll seldom have enough entities to bother with housekeeping. But please do consider that on occasion and sooner or later for most organizations you will come across more complicated models that you need to manage in a more sophisticated way. For those who don't use it most organizations designate some basic housekeeping rules that make use of layers for construction geometry and categories to provide labels for those layers. For the most part NX does a good job of automatically turning on the layers it needs to make visible the geometry needed to edit any feature that you select from the model navigator.
I'm not unaware that other CAD systems don't use layers e.g. just show and no-show. Some may have become used to it, but I find it the worst thing possible to have to deal with that in order to isolate the features that I need to work on I might be faced with a sea of intermingled features in trying to pick out the ones that I need. That is why I think that no matter what the final result becomes you need more that one filter to collect and manage entities so that you're quickly and easily able to isolate elements of your model especially when you have to manage construction geometry.
