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auto add to ref sets
- Thread starter moog2
- Start date
JohnRBaker
Mechanical
Go to File -> Customer Defaults -> Assemblies -> Site Standards -> Reference Sets and change the 'Contents' setting from 'Sheets and Solids' to 'Solid Priority', which means that if there are ONLY sheet bodies they will be included but as soon as the first solid be created it becomes the 'priority' member of the Model Reference Set and other object types will have to be explictly added.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
Shadowspawn
Aerospace
John,
How about the setting controling what/when solids are added? Currently, all bodies are added (even components) and I'd like to change it so that the user has to explicitly add the geom he wants. TIA...
Regards,
SS
CAD should pay for itself, shouldn't it?
How about the setting controling what/when solids are added? Currently, all bodies are added (even components) and I'd like to change it so that the user has to explicitly add the geom he wants. TIA...
Regards,
SS
CAD should pay for itself, shouldn't it?
Shadowspawn,
Why not use a custom reference set that you create (this can even be done by a grip program during file creation using a user exit)? This way the system has no control over the objects, the user will be responsible for entities in the set.
Why not use a custom reference set that you create (this can even be done by a grip program during file creation using a user exit)? This way the system has no control over the objects, the user will be responsible for entities in the set.
JohnRBaker
Mechanical
For one thing, we recommend, when asked, to never create Reference Sets in an Assembly. Granted, they do work, but if you're not careful they can come back and bite you as they act as 'filters', and I've seen people pull their hair out insisting that they keep adding components to a sub-assembly and wondering why they never show up at the top-level assembly only later to discover that somewhere along the chain from top level assembly down to the last sub-assembly that the user expected to see, was a Reference Set blocking the whole process. Thare are now other mechanisms much better suited to controlling the content of assemblies such as Arrangements and such, and if someone was using Reference Sets to control what is seen in Drawing views, we have tools implemented there for that purpose as well that are recommended, such as Hide Component in View (and don't confuse this with Visible in View as that's something we would really like to get people to stop using).
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
Shadowspawn
Aerospace
John, et al,
I think there's a misunderstanding somewhere. Currently, all solid bodies, regardless whether it's a component or not, is automatically added to the default ref set of the displayed/work part. Were not creating ref sets or adding anything to the default ref set outside of what the system does automatically. I currently have users remove everything from the ref set (at the detail part level) and explicitly add the desired geometry.
John, I whole heartedly agree with what you said above btw...
Regards,
SS
CAD should pay for itself, shouldn't it?
I think there's a misunderstanding somewhere. Currently, all solid bodies, regardless whether it's a component or not, is automatically added to the default ref set of the displayed/work part. Were not creating ref sets or adding anything to the default ref set outside of what the system does automatically. I currently have users remove everything from the ref set (at the detail part level) and explicitly add the desired geometry.
John, I whole heartedly agree with what you said above btw...
Regards,
SS
CAD should pay for itself, shouldn't it?
JohnRBaker
Mechanical
Yes, if the 'Solid Priority' is what has been set in Customer Defaults, all solid bodies will be automatically added to the Default 'Model' reference set. That is by design.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
(and don't confuse this with Visible in View as that's something we would really like to get people to stop using)
Please, please remove this function!! I detest it. I have a few stubborn co-workers who insist on using this to turn on and off layers. First they go to 'Visible in View', turn on the layers, then go to the layer dialog to turn them on. I tried showing them how the same can be accomplished with only the layer dialog, but to no avail. Nothing worse than opening a part when someone has screwed around with vis in view. The abuse of reference sets comes in a close second though.
-Derek
Please, please remove this function!! I detest it. I have a few stubborn co-workers who insist on using this to turn on and off layers. First they go to 'Visible in View', turn on the layers, then go to the layer dialog to turn them on. I tried showing them how the same can be accomplished with only the layer dialog, but to no avail. Nothing worse than opening a part when someone has screwed around with vis in view. The abuse of reference sets comes in a close second though.
-Derek
It is still needed in drafting, and probably fairly heavily relied upon for that to this day.
Visible in View goes back prior to UG version 10, where it was used as virtually the only way to create views that were added to a drawing, back when drawings were nothing much more than a fancy layout. So I guess it persisted so that old files could be opened without losing anything.
It was also the case way post version 10, that if you extracted silhouette curves they were made view dependent, and therein hangs another tale, that which is visible in view and that which is view dependent are really techniques that crossed over into the model side of things, so that the question becomes where should the two meet, and how can you get rid of anything that might support someone's "legacy data".
I dislike when people use it in modeling space, but I do see it used where text is added to layouts etc. It happens that we do see different groups of people who occasionally fall into using a technique that probably wasn't the intended use of the system. In automotive layouts they like to put text in model space, for example.
The real problem comes about when there are too many filters in play so that objects in the model can get really hard to find. If we're ever going to make progress in that department it would be nice in future versions if certain types of filter could be toggled on and off at will. So that you could turn off the ability of the system to hide visible in view objects for a time, and then re-enable that filter type if you need to when you're done cleaning up.
Just a thought,
Regards
Hudson
Visible in View goes back prior to UG version 10, where it was used as virtually the only way to create views that were added to a drawing, back when drawings were nothing much more than a fancy layout. So I guess it persisted so that old files could be opened without losing anything.
It was also the case way post version 10, that if you extracted silhouette curves they were made view dependent, and therein hangs another tale, that which is visible in view and that which is view dependent are really techniques that crossed over into the model side of things, so that the question becomes where should the two meet, and how can you get rid of anything that might support someone's "legacy data".
I dislike when people use it in modeling space, but I do see it used where text is added to layouts etc. It happens that we do see different groups of people who occasionally fall into using a technique that probably wasn't the intended use of the system. In automotive layouts they like to put text in model space, for example.
The real problem comes about when there are too many filters in play so that objects in the model can get really hard to find. If we're ever going to make progress in that department it would be nice in future versions if certain types of filter could be toggled on and off at will. So that you could turn off the ability of the system to hide visible in view objects for a time, and then re-enable that filter type if you need to when you're done cleaning up.
Just a thought,
Regards
Hudson
JohnRBaker
Mechanical
Hudson pretty well covered the reason why some of these 'legacy' functions havn't been removed completely, but that still should not mean that these can be used as part of a valid workflow today, since as Hudson and others have mentioned, we have implemented superior tools for doing most of these things. And one of the more recent capabilities, to help overcome the issue of using (or should I say misusing) Drafting functions in modeling, is the introduction of PIM, where you can 'document' and 'annotate' the 3D model using what looks like drafting objects such as dimensions, GD&T symbology, notes, labels, crosshatching, sectioning, etc, but all in the context of the 3D model so that these non-geometric objects become part of the product design.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
I'd like to see "Visible in View" disabled in Modeling, but I still see a use for it in Drafting. But, that said, if there is a better way to accomplish my scenario below, without using Visible in View, I'd like to hear it.
We have our drawings, and models in the same file...I know, it's not the master model way, but I have had no luck in convincing anyone that separate model and drawing files are better, plus we have a lot of legacy files done this way. Anyway, many times we'll have more than one solid, and each needs to be detailed separate, and then shown as a welded assembly. We *could* make each piece a separate file, but I know I'd never convince anyone that would be better, and in most cases I think it would slow us down. ViV is the only way I know of, to show each part by itself to detail it, and show all the parts together, within the same file.
-Dave
-Dave
Everything should be designed as simple as possible, but not simpler.
We have our drawings, and models in the same file...I know, it's not the master model way, but I have had no luck in convincing anyone that separate model and drawing files are better, plus we have a lot of legacy files done this way. Anyway, many times we'll have more than one solid, and each needs to be detailed separate, and then shown as a welded assembly. We *could* make each piece a separate file, but I know I'd never convince anyone that would be better, and in most cases I think it would slow us down. ViV is the only way I know of, to show each part by itself to detail it, and show all the parts together, within the same file.
-Dave
-Dave
Everything should be designed as simple as possible, but not simpler.
JohnRBaker
Mechanical
For every situation there's an exception and what you described is probably the classic one for at least keeping Visible-in-view around for Drafting purposes.
As for disabling Visible-in-view in Modeling, you can do the next best thing. Just go into Modeling, then open the Customization dialog, pull down the Format menu and select and drag the 'Visible-in-view' item off into the middle of the screen and 'drop' it. Then do the same thing with the Icon off the Utility toolbar. And if your people have been using the keyboard shortcut, you'll have to remove that as well. Then save your role and load it on all of your users seats.
Now this will only make it impossible to run Visible-in-view in modeling (if you can't find the menu item/icon, you can't use the function) as it will still be available in Drafting.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
As for disabling Visible-in-view in Modeling, you can do the next best thing. Just go into Modeling, then open the Customization dialog, pull down the Format menu and select and drag the 'Visible-in-view' item off into the middle of the screen and 'drop' it. Then do the same thing with the Icon off the Utility toolbar. And if your people have been using the keyboard shortcut, you'll have to remove that as well. Then save your role and load it on all of your users seats.
Now this will only make it impossible to run Visible-in-view in modeling (if you can't find the menu item/icon, you can't use the function) as it will still be available in Drafting.
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
Oh John,
That is nasty there are some people we definitely have to do that to when we get the chance. Like the minute their backs are turned![[thumbsup]](/data/assets/smilies/thumbsup.gif "[thumbsup] [thumbsup]")
. That is to stop them from using visible in view ![[wink]](/data/assets/smilies/wink.gif "[wink] [wink]")
Dave,
The reason given for using the master model concept and for using assemblies, is that at some point you will find yourself loading more data than you need to look at a specific area of your design. This is where partial loading comes in to some extent. If your model contains a drawing then that file is bigger for carrying with it the extra data. So at some stage when you open an assembly and need to fully open components so that your wave linking and mating will be 100% manifest, then you'll be loading some data into memory that you just don't need. This is part of the case to be made for using master model, and separating the drawings from the models.
I've talked about this quite a lot in the past in the vein of arguing that there is and should be a clear design intent that flows through from the way the NX software is written to the way it can be used, so that it is the right tool for the job, giving you the best result when you use it properly. This is not to criticize you in any way, rather I'd like you to have a better experience of using CAD by helping you convince others to come into the light. Armed with a bit of knowledge about what is possible you might go be able to go back to them and say NX has all these wonderful tools that make life easier and save time, and we just aren't using it to best advantage.
One big thing is drawing templates that basically only work to best advantage if you use master model concept. You can really have your cake and eat it with these. I'm making drawings in minutes not hours, because I have learned how to do a few steps in customizing the system that save me hours of work later on.
By the way there is yet another reason why separating drawing and model works for many organizations that has to do with releasing and revising your designs. If kept separate the model and drawing can be at different release levels, so that you may choose to change either several times without revising the other and your system can be set up to reflect that activity.
Best Regards
Hudson
That is nasty there are some people we definitely have to do that to when we get the chance. Like the minute their backs are turned
. That is to stop them from using visible in view Dave,
The reason given for using the master model concept and for using assemblies, is that at some point you will find yourself loading more data than you need to look at a specific area of your design. This is where partial loading comes in to some extent. If your model contains a drawing then that file is bigger for carrying with it the extra data. So at some stage when you open an assembly and need to fully open components so that your wave linking and mating will be 100% manifest, then you'll be loading some data into memory that you just don't need. This is part of the case to be made for using master model, and separating the drawings from the models.
I've talked about this quite a lot in the past in the vein of arguing that there is and should be a clear design intent that flows through from the way the NX software is written to the way it can be used, so that it is the right tool for the job, giving you the best result when you use it properly. This is not to criticize you in any way, rather I'd like you to have a better experience of using CAD by helping you convince others to come into the light. Armed with a bit of knowledge about what is possible you might go be able to go back to them and say NX has all these wonderful tools that make life easier and save time, and we just aren't using it to best advantage.
One big thing is drawing templates that basically only work to best advantage if you use master model concept. You can really have your cake and eat it with these. I'm making drawings in minutes not hours, because I have learned how to do a few steps in customizing the system that save me hours of work later on.
By the way there is yet another reason why separating drawing and model works for many organizations that has to do with releasing and revising your designs. If kept separate the model and drawing can be at different release levels, so that you may choose to change either several times without revising the other and your system can be set up to reflect that activity.
Best Regards
Hudson
Hudson,
Oh, I know the reasons
but convincing the rest of the (less experienced) design department is not an easy task. This is the first place I've ever worked, that does not use the master model concept.
The battle goes on...but I am slowlyl bringing them around.
-Dave
-Dave
Everything should be designed as simple as possible, but not simpler.
Oh, I know the reasons
but convincing the rest of the (less experienced) design department is not an easy task. This is the first place I've ever worked, that does not use the master model concept. The battle goes on...but I am slowlyl bringing them around.
-Dave
-Dave
Everything should be designed as simple as possible, but not simpler.
Yes Dave,
I've worked through your situation and different companies two or three times in the past and it is always a struggle to bring them out of the dark ages. The typical cycle is that they set out to do engineering starting with something basic like Autocad, and then realize that they need a decent CAD system. Often there is an intermediate step where they try to save money and go for Solid edge or worse, then they either go to NX because they see the light or because they've been swallowed up by a corporation that already has NX. At this stage you've got a few engineers who think they're the smartest guys in the office but shun the CAD because they just don't get it, and under them are a bunch of users with too much to learn in too little time. So what they do is employ somebody who actually knows what they're talking about and then hesitate to listen to you because you're an outsider.
You don't need me you need Machaavelli.
Anyway I somewhat sympathize, so that's why I wrote.
Best of Luck
Hudson
I've worked through your situation and different companies two or three times in the past and it is always a struggle to bring them out of the dark ages. The typical cycle is that they set out to do engineering starting with something basic like Autocad, and then realize that they need a decent CAD system. Often there is an intermediate step where they try to save money and go for Solid edge or worse, then they either go to NX because they see the light or because they've been swallowed up by a corporation that already has NX. At this stage you've got a few engineers who think they're the smartest guys in the office but shun the CAD because they just don't get it, and under them are a bunch of users with too much to learn in too little time. So what they do is employ somebody who actually knows what they're talking about and then hesitate to listen to you because you're an outsider.
You don't need me you need Machaavelli.
Anyway I somewhat sympathize, so that's why I wrote.
Best of Luck
Hudson
- Thread starter
- #17
Dave,
Well almost. In writing that I reminded myself of the character Hawkeye Pierce, played by Alan Alda in an episode of M*A*S*H where he described to a wounded soldier all the familiar things about his home town in order to cheer the guy up. When asked out of earshot how he new so much about Hicksville Nebraska, he simply replied that he'd just described every small town in America, and let imagination do the rest.
If anybody has seen the UK comedy "The Office", with Ricky Gervase, then you get the same thing there. I actually worked in one of these places where my boss fell of his chair in his sleep! It doesn't get much funnier than that![[smile]](/data/assets/smilies/smile.gif "[smile] [smile]")
.
Seriously these thing happen because human nature is what it is and events occur for structural reasons in the life cycle of many organizations that bring them to a similar point. You who have the benefit of education and experience can see that because you have attained the same vantage point as one another, hopefully it means you can make a bit of a dent in the ignorance that surrounds us as well.
Best regards
Hudson
Well almost. In writing that I reminded myself of the character Hawkeye Pierce, played by Alan Alda in an episode of M*A*S*H where he described to a wounded soldier all the familiar things about his home town in order to cheer the guy up. When asked out of earshot how he new so much about Hicksville Nebraska, he simply replied that he'd just described every small town in America, and let imagination do the rest.
If anybody has seen the UK comedy "The Office", with Ricky Gervase, then you get the same thing there. I actually worked in one of these places where my boss fell of his chair in his sleep! It doesn't get much funnier than that
.Seriously these thing happen because human nature is what it is and events occur for structural reasons in the life cycle of many organizations that bring them to a similar point. You who have the benefit of education and experience can see that because you have attained the same vantage point as one another, hopefully it means you can make a bit of a dent in the ignorance that surrounds us as well.
Best regards
Hudson
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