Regeneration (update) Order 1

[NXMold]

In ProE the regeneration order was pretty obvious, it started at the top of the tree and stepped through until the bottom. Thats it.

UG is a little more interesting I see, in a single part it updates after each change (it seems) and I can only guess that it goes through the part navigator items in order like proe did, with the addition of unparameterized features.

What I don't get is what happens with assemblies. I work with generally 40-200 part assemblies (not counting multiple instances) with quite a fair bit of interpart modeling (wave linked, and expressions). Everything works just fine until..... I add mating conditions.

Let the circular references fly! So far I have avoided mating, but that Will be changing very soon. My previously acceptable modeling practices no longer work, and I suspect it has to do with regen.. updating the other parts in an assembly after a change, then that update causing the other part to update...

I don't get the order as it applies to wave linking and mating. If I need to give a more specific example I can.

 

[JohnRBaker]

What version are you running? When you move to NX 5, you'll have the option of using Assembly Constraints (instead of Mating Conditions) which are NOT order sensitive and reduces, and in many cases completely eliminates, circular reference problems.


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]

For what it is worth it can be a matter of how you use mating conditions, if you're going to use them. I have worked with them quite happily for adding fasteners, because if you're dealing with a bolt hole array then you get to install all the fasteners in one step. Other than that I often pick and choose where and when I want to use mating conditions.

A lot of people design all their parts, except fasteners, about an absolute co-ordinate system for their project, where few parts are likely to be interchangeable between different products. In that case you may choose not to use mating conditions unless there is a particular articulation of parts that you need to be able to perform in order to demonstrate or analyze a range of motion.

The reason that I mention this in connection with your question is that we have found in the past that very large numbers of mating conditions can be quite burdensome to maintain, and really drag down performance. Most sites I have encountered who adopt a mindset that everything has to be mated give it away once their product becomes sufficiently complex that it starts to bite.

Best regards

Hudson

 

[NXMold]

Forgot to mention that, NX 5.0.2

I'm also using Mold Wizard, and that system does not use any mating at all but rather tries to control position with interpart expressions based on the ACS. What really bites is changing plate sizes/locations and then having to go and manually update the position and size of so bloody many parts. I've got to automate that and capture design intent! None of my parts are used in multiple designs (except library components, but thats a different topic).

In my class, the instructor cautioned us about Assembly Constraints, and sure enough 2/3rds of the class computers crashed during that excercise. More than once. Hopefully thats being worked out.

 

[NXMold]

I’m a new user with just a couple hundred hours on NX 5.0.2, here are some of my notes/questions/er’s (probably not all relevant to this thread)

1) We have measure radius, where is measure diameter? The current tool should output both.
2) Update display should happen after rotating! Tough to see silhouette edges in NX
3) I want to add sketch constraints using the Action -> Object method
4) Many (most?) of us use dual monitors, it would be nice to dock things outside the main application window like the assy navigator and part navigator. Dual monitors need to be supported by UGS.
5) When docking toolbars vertically on the left or right, they cannot be stacked one above the other. This wastes space.
6) I’d like to be able to create datum planes while a feature dialog is open
7) Why does the point constructor for the hole dialog open inside a sketch? This would make more sense if you could use sketch constraints and dimensions on the points, but the points don’t appear to be sketch entities?
8) Make the world a better place, destroy the layers!
9) OK, Apply, and Cancel are not descriptive, and behave inconsistently.
10) I’d like a toggle option to include the boundary faces in the region of faces selection
11) Drop down list in selection bar could be lengthened to prevent or reduce scrolling
12) How do you specify a different draft angle for each side of a selected edge?
13) What is the difference between linking a composite curve and a sketch?
14) Need a quicker shortcut button to “Display parent” without using the context menu flyout
15) Mating conditions easily cause circular references, how and why is that? What order does the model update in?

 

[NXMold]

Oops, I meant to post that in the big long "fix that" thread

 

[JohnRBaker]

Disclaimer, all of my responses below are with respect to NX 5.0.2.2 unless stated otherwise.

1) We have measure radius, where is measure diameter? The current tool should output both.

Except in terms of the diameter of something like a hole feature which is stored as a parameter, when CAD systems measure values, like the face of a solid, they query the data structure of the geometric object and in the case of cylindrical faces and arcs/circles, only the radius is stored in the object record. Granted, we could 'derive' the diameter, but that's not the data that's stored with this class of objects.

2) Update display should happen after rotating! Tough to see silhouette edges in NX

If you're truly a new user of NX, someone must have gotten you off on the wrong foot. With NX 5, out-of-the-box, the so-called wireframe display of the model will automatically update as you rotate the display. To get the display to show what it sounds like you're using, that is 'static wireframe', you would have to either explictly select that mode from a menu or you'd have to add the Icon to the View toolbar. I would advise that you stick to 'Wireframe with Hidden Edges' or 'Wireframe with Dim Edges' since those will behave as you would like them to.

3) I want to add sketch constraints using the Action -> Object method

I'm not sure what you mean here? You have the choice of either selecting a series of sketch curves and then press MB3 and select 'Add Constraints', which would be Object -> Action. Or you could go to the Sketch COnstraints toolbar and select the 'Constraints' icon and then select the curves of interest, which would be Action -> Object. Granted, we don't display a list of available constraints until you select one or more curves, but that is so that we only offer you constraint options that would be valid for the set of curves that you've selected as well as allowing us to indicate if certain constraint conditions already exist for the cirves selected (they're the items that are 'depressed' and grayed-out).

4) Many (most?) of us use dual monitors, it would be nice to dock things outside the main application window like the assy navigator and part navigator. Dual monitors need to be supported by UGS.

Many of those limitations are due to issues with respect to Windows and the Open GL graphics standards. Note that originally NX was NOT developed with dual-screen support as part of our requirements for the product, but we have gotten requests to make what level of support we do provide better and there is work being done in future releases which will provide better support.

5) When docking toolbars vertically on the left or right, they cannot be stacked one above the other. This wastes space.

I don't know what your problem is, but I have NO issues whatsoever with stacking more than one toolbar vertically in the same 'column'.

6) I’d like to be able to create datum planes while a feature dialog is open

Functions that can be executed while another dialog is open and not cancel the original operation are called 'special functions'. Unfortunately, there is no architectural support for creating parametric features as part of a 'special function'. However, for those functions where it's likely that a user might need to reference an existing Datum, we are gradually adding options to perform that task from the existing dialog itself as can be seen in the first dialog displayed when you create a Sketch or when performing a Trim Body. Also, many functions are allowing you to define a plane on the fly. Granted, these are not created as separate features, but are defined as part of the feature itself. For an example of that approach, look at Instance Geometry (Mirror).

7) Why does the point constructor for the hole dialog open inside a sketch? This would make more sense if you could use sketch constraints and dimensions on the points, but the points don’t appear to be sketch entities?

The points created inside the Sketcher as part of the new Hole function are just like any other sketch object which means that they can be constrained, dimensioned, whatever. Once you enter that sketch mode, YOU'RE in the full sketcher, period. All sketch functions are available to you, it's just that the DEFAULT mode is creating points, but you can change that by just selecting another function. For example, it might be easier to create rectangle, dimensions it and place 4 points, one constrained at each corner, as the hole locations. Or you could just create 4 points and dimension them directly. It's up to you as you have all the tools of the sketcher at your fingertips.

8) Make the world a better place, destroy the layers!

Trust me, I'd be the first person in line to throw the switch on that one myself. Unfortunately, we have thousands of customers who have been using UG/NX for years (I've got over 30 years of experience myself) and many of them have data standards and applications and workflows that depend on layers, and while I personally have weened myself off of them and use other schemes to control the display of my working models, for our very largest customers, that's just not a practical expectations. But that being said, no one is FORCING you to use them and I'm aware of no function or opeation that requires you to have a more than one layer active and visible. So just use Customize and remove all of the Layer icons and menus from your interface. Problem solved ;-)

9) OK, Apply, and Cancel are not descriptive, and behave inconsistently.

But they are traditional and are an intergral part of our interface style. As for consistency, as we move all of the dialogs to the new NX 5 style, their behavior and action will become much more consistent.

10) I’d like a toggle option to include the boundary faces in the region of faces selection

I'm going to need more information and perhaps even an example of where and why this is an issue.

11) Drop down list in selection bar could be lengthened to prevent or reduce scrolling

You have to make certain compromies since LONG lists are both scary and requires lots of mouse travel, which is generally mitigated to some extent with scrolled windows, however, I suspect that I know what you're complaint is being directed at and that's the Selection Filter list. Part of the problem is that we are updating more and more functions to use the general selection tools so this list has grown over time, however, when inside of a dialog, that list is generally much shorter and often does not require a scrolling list.

12) How do you specify a different draft angle for each side of a selected edge?

I assume that you're talking about when you're creating an extrude feature and using the draft option. Well once you have the preview on the screen, go to the Draft section of the dialog and in select the Draft option 'From Section' and then select the 'Angle Option' of 'Multiple'. Now you will have the option to define a different draft angle for each segment of the extrude profile.

13) What is the difference between linking a composite curve and a sketch?

When you select a Sketch, you are, by definition, selecting multiple curves as a single object. However, if you're not selecting a sketch but a series if individual curves, we treat them as if they were a single or composite curve. It's as if you first had used the Join Curve function to create what many people would call a 'composite curve' (actually we create a spline which is linked associatively to the original set of curves which are unchanged).

14) Need a quicker shortcut button to “Display parent” without using the context menu flyout

An extra button here, and extra button there, pretty soon you've got a UI that looks way too complicated for most people. We have to depend on common, simple, easy to understand, approaches and then use them over and over again and the use of selecting an object and then use MB3 to get to options, is pervasive through out NX and represents thousands of additional opertions and options that does NOT require explicit buttons and icons.

15) Mating conditions easily cause circular references, how and why is that? What order does the model update in?

If you using NX 5, you are you still using Mating COnditions. Get with the program and move to Assembly Constraints. I suspect that most all of your issues will be history.


Anyway, I hope this long reply to your long list will help you move forward with your use of NX.


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]

John,

I have don't have a sense of the method that you would use to do away with layers. Some models require a great deal of construction geometry including curves, trim sheets and sketches. It is handy to be able to use layers to filter out that geometry. The only other filters that I know of are blanking, combinations of visible in view and view dependency, and reference sets. Have I left any out? What else to you prefer to use as an alternative to layers?

I'll go first.
Blanking or its equivalent was the only thing available in older versions of Catia, and I hated that, combined with the fact that it just forced you to use keep too many entities in the file. To me blanking as a filter is equivalent to having only two layers and that just isn't enough.

The use of reference sets is theoretically an option, but since they only make sense in the context of an assembly that does nothing to manage your data if you're working in the component.

Visible in view or view dependency for objects in modeling has become a bit of a pet hate. We needed to use it back in the good ol' days pre version 9 to set up drawing views, but it has become an seldom used extra way to hide entities where they become difficult to find. The typical situation is where 99 entities exist on layer 200, but you have to guess which view they've been hidden in.
Just as you described the situation where it would be possible to ignore the existence of layers so too there are probably ways to adapt your methods to use view based filters as an alternative. The problem is that if you want to get rid of layers then there needs to be an alternative and I would like to know what you propose.

BTW
I agree with most of your other responses above. It is interesting to me to hear what users bring up in terms of how they want to use NX, in ways that come from either other CAD systems or purely from fertile imaginations, (I mean that in a good way).
I think that there is a difference between a fully functional system that has an intended method to achieve the maximum number of tasks, as opposed to a proliferation of ways to do the same things with different methods some of which don't really sit well in the scheme of things. At the heart of that argument there must be a nexus between core functionality and non-core customization, so that the system does the simplest most frequent operations the best way by default and defers to other embellishments as required, last used, or by customization, (ticking something or or off).

Most of the time it works like this and does pretty well.

One part of me likes to display every available icon and have maximum choice to do as I wish, while another part wants desperately to cull the system back to what is necessary and drive some uniformity into the way people work so the system is easier to teach/learn and to maintain the data. At the end of the say I'm happy to have the ability to do almost anything, just as long as it doesn't have to be instead of core functionality. Nor do I want to clutter dialogs with extended methods at the expense of having to manage to avoid parts of the dialog which I'm not using. In the past we have had the ability to turn icons on and off, I favor the dialogs with a pull down panel for extended options, which can be avoided most of the time. I think some more of that would work to good effect for a lot of the extended methods that users often propose.

Best Regards

Hudson

 

[NXMold]

WOW, I didn’t expect such a detailed and helpful reply, much appreciated! Let me expand a little… (I’ll mark my new responses in bold in case that’s not clear).

----------
Disclaimer, all of my responses below are with respect to NX 5.0.2.2 unless stated otherwise.

1) We have measure radius, where is measure diameter? The current tool should output both.

Except in terms of the diameter of something like a hole feature which is stored as a parameter, when CAD systems measure values, like the face of a solid, they query the data structure of the geometric object and in the case of cylindrical faces and arcs/circles, only the radius is stored in the object record. Granted, we could 'derive' the diameter, but that's not the data that's stored with this class of objects.

I understand, but I’m spending a lot of time running to my calculator checking metric vs inch component and clearance diameters against catalogs etc… everything I do is based on diameters. Other cad systems offer this information.

2) Update display should happen after rotating! Tough to see silhouette edges in NX

If you're truly a new user of NX, someone must have gotten you off on the wrong foot. With NX 5, out-of-the-box, the so-called wireframe display of the model will automatically update as you rotate the display. To get the display to show what it sounds like you're using, that is 'static wireframe', you would have to either explictly select that mode from a menu or you'd have to add the Icon to the View toolbar. I would advise that you stick to 'Wireframe with Hidden Edges' or 'Wireframe with Dim Edges' since those will behave as you would like them to.

Correct, I am using static wireframe. This is because silhouette edges are not shown at all in ‘wireframe with dim edges’. With lots of cylindrical features and holes, silhouette edges are very important to me. I have gone to Visualization Preferences, Visual, Edge display settings, and the silhouettes check box is only available in static wireframe. It has no effect on WF with dim edges.

3) I want to add sketch constraints using the Action -> Object method

I'm not sure what you mean here? You have the choice of either selecting a series of sketch curves and then press MB3 and select 'Add Constraints', which would be Object -> Action. Or you could go to the Sketch Constraints toolbar and select the 'Constraints' icon and then select the curves of interest, which would be Action -> Object. Granted, we don't display a list of available constraints until you select one or more curves, but that is so that we only offer you constraint options that would be valid for the set of curves that you've selected as well as allowing us to indicate if certain constraint conditions already exist for the cirves selected (they're the items that are 'depressed' and grayed-out).

It would be faster in some cases to select the constraint and then pick all the entities in a sketch to apply it to.

4) Many (most?) of us use dual monitors, it would be nice to dock things outside the main application window like the assy navigator and part navigator. Dual monitors need to be supported by UGS.

Many of those limitations are due to issues with respect to Windows and the Open GL graphics standards. Note that originally NX was NOT developed with dual-screen support as part of our requirements for the product, but we have gotten requests to make what level of support we do provide better and there is work being done in future releases which will provide better support.
That’s good!

5) When docking toolbars vertically on the left or right, they cannot be stacked one above the other. This wastes space.

I don't know what your problem is, but I have NO issues whatsoever with stacking more than one toolbar vertically in the same 'column'.

I don’t know why, but it does not allow me to. See attached picture 5a.gif, I cannot put these in a vertical column (using the essentials role for an example)

6) I’d like to be able to create datum planes while a feature dialog is open

Functions that can be executed while another dialog is open and not cancel the original operation are called 'special functions'. Unfortunately, there is no architectural support for creating parametric features as part of a 'special function'. However, for those functions where it's likely that a user might need to reference an existing Datum, we are gradually adding options to perform that task from the existing dialog itself as can be seen in the first dialog displayed when you create a Sketch or when performing a Trim Body. Also, many functions are allowing you to define a plane on the fly. Granted, these are not created as separate features, but are defined as part of the feature itself. For an example of that approach, look at Instance Geometry (Mirror).

Good to see this support increasing, coming from ProE I notice I have to cancel a lot more feature dialogs to back track and create a plane, or show/hide, or whatever. The dialogs really lock you out of NX, though I’m sure I’ll notice it less as I adapt.

7) Why does the point constructor for the hole dialog open inside a sketch? This would make more sense if you could use sketch constraints and dimensions on the points, but the points don’t appear to be sketch entities?

The points created inside the Sketcher as part of the new Hole function are just like any other sketch object which means that they can be constrained, dimensioned, whatever. Once you enter that sketch mode, YOU'RE in the full sketcher, period. All sketch functions are available to you, it's just that the DEFAULT mode is creating points, but you can change that by just selecting another function. For example, it might be easier to create rectangle, dimensions it and place 4 points, one constrained at each corner, as the hole locations. Or you could just create 4 points and dimension them directly. It's up to you as you have all the tools of the sketcher at your fingertips.

8) Make the world a better place, destroy the layers!

Trust me, I'd be the first person in line to throw the switch on that one myself. Unfortunately, we have thousands of customers who have been using UG/NX for years (I've got over 30 years of experience myself) and many of them have data standards and applications and workflows that depend on layers, and while I personally have weened myself off of them and use other schemes to control the display of my working models, for our very largest customers, that's just not a practical expectations. But that being said, no one is FORCING you to use them and I'm aware of no function or opeation that requires you to have a more than one layer active and visible. So just use Customize and remove all of the Layer icons and menus from your interface. Problem solved

Got it, although mold wizard creates a lot of layers so I might be stuck with them anyway. I liked that ProE offered toolbar buttons to hide Planes, Axis, Points, and Cys globally in your current application (in addition to show/hide and layers). You could leave some primary datums naked in the model, not on any layers at all, with the dozens of construction datums hidden on layers. Then you could always easily show the primary datums. No matter, there are lots of ways to accomplish this with NX.

9) OK, Apply, and Cancel are not descriptive, and behave inconsistently.

But they are traditional and are an intergral part of our interface style. As for consistency, as we move all of the dialogs to the new NX 5 style, their behavior and action will become much more consistent.

Just a general non-NX windows rant then I guess, but sometimes Dismiss, Continue, or other terms would be SO MUCH clearer than “Press YES for cancel and NO to apply with warnings” (or whatever).

10) I’d like a toggle option to include the boundary faces in the region of faces selection

I'm going to need more information and perhaps even an example of where and why this is an issue.

Ah, this one is interesting for sure. When picking a region of faces on a complex part, sometimes there is a ‘break point’ in the model that allows you to pick just four or five surfaces to define the boundry, but those surfaces belong with the region you are copying. In order to include them, I’d have to pick a different set in the complex area (maybe 150 surfaces instead of 5, which is impractical). Sure I can make a second extract for those 5 boundry surfaces, then sew, but it would be nice to have the option to include the boundry surfaces in the extracted region or not, since I’ve already gone to the trouble to pick them. Additionally, it would be nice to have the option of adding or removing a couple other surfaces manually. The ProE equivalent that I am accustomed to used seed/boundary just as a selection method during the surface copy.

11) Drop down list in selection bar could be lengthened to prevent or reduce scrolling

You have to make certain compromies since LONG lists are both scary and requires lots of mouse travel, which is generally mitigated to some extent with scrolled windows, however, I suspect that I know what you're complaint is being directed at and that's the Selection Filter list. Part of the problem is that we are updating more and more functions to use the general selection tools so this list has grown over time, however, when inside of a dialog, that list is generally much shorter and often does not require a scrolling list.

Yes, the selection filter list. Particularly points and planes require a lot of mouse work due to scrolling, but I understand the compromise.

12) How do you specify a different draft angle for each side of a selected edge?

I assume that you're talking about when you're creating an extrude feature and using the draft option. Well once you have the preview on the screen, go to the Draft section of the dialog and in select the Draft option 'From Section' and then select the 'Angle Option' of 'Multiple'. Now you will have the option to define a different draft angle for each segment of the extrude profile.

No, I’m using the draft feature on imported geometry (mostly) with the ‘from edges’ type. It will draft both cavity and core side at the same angle, but I need to input different angles for each side. In some cases I have been able to work around by being sneaky with my edge selection to eliminate faces on one side, then apply a second draft feature.

13) What is the difference between linking a composite curve and a sketch?

When you select a Sketch, you are, by definition, selecting multiple curves as a single object. However, if you're not selecting a sketch but a series if individual curves, we treat them as if they were a single or composite curve. It's as if you first had used the Join Curve function to create what many people would call a 'composite curve' (actually we create a spline which is linked associatively to the original set of curves which are unchanged).

I think I understand, but I’m confused because wouldn’t link composite curve with ‘feature curves’ accomplish the same thing? Picking a sketch is really a selection method, not a different feature type? Are the results the same with my method?

14) Need a quicker shortcut button to “Display parent” without using the context menu flyout

An extra button here, and extra button there, pretty soon you've got a UI that looks way too complicated for most people. We have to depend on common, simple, easy to understand, approaches and then use them over and over again and the use of selecting an object and then use MB3 to get to options, is pervasive through out NX and represents thousands of additional opertions and options that does NOT require explicit buttons and icons.

Hmm…. I spend an awful lot of time switching between levels of assemblies, and the context menu flyout (especially if I have to depend on the resource bar assembly navigator flyout!) slows me down. This one would save measureable time in my day. Bury it in the Assemblies, context control menu and I'll put it right up front in my customer toolbar!

15) Mating conditions easily cause circular references, how and why is that? What order does the model update in?

If you using NX 5, you are you still using Mating COnditions. Get with the program and move to Assembly Constraints. I suspect that most all of your issues will be history.

Anyway, I hope this long reply to your long list will help you move forward with your use of NX.
----------

THANK YOU again for your detailed response, it is very helpful.

A note regarding icons and customization, I LOVE that everything is available in the top menu bar in a (largely) consistent and accessible manner, and then the icons are customized beyond recognition per user, or mood, to be quicker to access. NX5 is a wonderful relief from Proe in most ways, while there are things I miss I wouldn’t want to go back! I’m also glad I didn’t have to learn in NX3 or earlier, the NX5 dialogs are fan-freakin-tastic and really make my day.

 

[JohnRBaker]

2) Update display should happen after rotating! Tough to see silhouette edges in NX

If you're truly a new user of NX, someone must have gotten you off on the wrong foot. With NX 5, out-of-the-box, the so-called wireframe display of the model will automatically update as you rotate the display. To get the display to show what it sounds like you're using, that is 'static wireframe', you would have to either explictly select that mode from a menu or you'd have to add the Icon to the View toolbar. I would advise that you stick to 'Wireframe with Hidden Edges' or 'Wireframe with Dim Edges' since those will behave as you would like them to.

Correct, I am using static wireframe. This is because silhouette edges are not shown at all in ‘wireframe with dim edges’. With lots of cylindrical features and holes, silhouette edges are very important to me. I have gone to Visualization Preferences, Visual, Edge display settings, and the silhouettes check box is only available in static wireframe. It has no effect on WF with dim edges.

That's true, the scheme that supports dynamic verse static-wireframe uses the shading buffers and as such can't distingish (at least not yet) internal silhouettes. Perhaps if you worked with shading ON, but with a translucency set to say 50% might be better.

3) I want to add sketch constraints using the Action -> Object method

I'm not sure what you mean here? You have the choice of either selecting a series of sketch curves and then press MB3 and select 'Add Constraints', which would be Object -> Action. Or you could go to the Sketch Constraints toolbar and select the 'Constraints' icon and then select the curves of interest, which would be Action -> Object. Granted, we don't display a list of available constraints until you select one or more curves, but that is so that we only offer you constraint options that would be valid for the set of curves that you've selected as well as allowing us to indicate if certain constraint conditions already exist for the cirves selected (they're the items that are 'depressed' and grayed-out).

It would be faster in some cases to select the constraint and then pick all the entities in a sketch to apply it to.

But then we would have to put more checks/masks and probably even more warning messages in the code when you tried picking objects not valid for the particular constraint scheme selected. Besides, with the current approach, I can define Multiple constraints in one operation, such as selecting 2 lines and making them both Equal Length and Vertical for example.

5) When docking toolbars vertically on the left or right, they cannot be stacked one above the other. This wastes space.

I don't know what your problem is, but I have NO issues whatsoever with stacking more than one toolbar vertically in the same 'column'.

I don’t know why, but it does not allow me to. See attached picture 5a.gif, I cannot put these in a vertical column (using the essentials role for an example)

I don't know what to say as I've never had that problem, although I have to admit that you're not the first to complain about this so perhaps there is an issues some where, but it might not be NX's fault but perhaps something in the Windows setup.

6) I’d like to be able to create datum planes while a feature dialog is open

Functions that can be executed while another dialog is open and not cancel the original operation are called 'special functions'. Unfortunately, there is no architectural support for creating parametric features as part of a 'special function'. However, for those functions where it's likely that a user might need to reference an existing Datum, we are gradually adding options to perform that task from the existing dialog itself as can be seen in the first dialog displayed when you create a Sketch or when performing a Trim Body. Also, many functions are allowing you to define a plane on the fly. Granted, these are not created as separate features, but are defined as part of the feature itself. For an example of that approach, look at Instance Geometry (Mirror).

Good to see this support increasing, coming from ProE I notice I have to cancel a lot more feature dialogs to back track and create a plane, or show/hide, or whatever. The dialogs really lock you out of NX, though I’m sure I’ll notice it less as I adapt.

Note you do NOT need to ever 'Cancel' out of a dialog, just select the next one that you desire. If it's a special function, such as Show/Hide, while you original dialog will disappear, it will reappear after you leave the special function. And if it's NOT a special function, it will automatically Cancel your old dialog before it displays its own.

8) Make the world a better place, destroy the layers!

Trust me, I'd be the first person in line to throw the switch on that one myself. Unfortunately, we have thousands of customers who have been using UG/NX for years (I've got over 30 years of experience myself) and many of them have data standards and applications and workflows that depend on layers, and while I personally have weened myself off of them and use other schemes to control the display of my working models, for our very largest customers, that's just not a practical expectations. But that being said, no one is FORCING you to use them and I'm aware of no function or opeation that requires you to have a more than one layer active and visible. So just use Customize and remove all of the Layer icons and menus from your interface. Problem solved

Got it, although mold wizard creates a lot of layers so I might be stuck with them anyway. I liked that ProE offered toolbar buttons to hide Planes, Axis, Points, and Cys globally in your current application (in addition to show/hide and layers). You could leave some primary datums naked in the model, not on any layers at all, with the dozens of construction datums hidden on layers. Then you could always easily show the primary datums. No matter, there are lots of ways to accomplish this with NX.

(This reply is for both NXMold and Hudson)

Starting with NX 5 we added a new 'Show and Hide' tool which allows you to control the global display of classes of objects, such as All Datums Planes, All Sketches, etc. (See the Image refernced below) Note that the list of avialble classes of objects will only show those that are actually in your model and on displayable layers (so this does NOT mess up any layering schemes that you are using). What you do is select the '+' to Show objects in that class, or '-' to Hide them. This should really help those people who would like to start to organize their models around a 'Show/Hide' approach rather than layers.

Also in Drafting, we've enhanced the selection of Components and Views for the 'Remove Component from View' function so as to make that more practical as well, again to help people who have chosen to move away from layers.

10) I’d like a toggle option to include the boundary faces in the region of faces selection

I'm going to need more information and perhaps even an example of where and why this is an issue.

Ah, this one is interesting for sure. When picking a region of faces on a complex part, sometimes there is a ‘break point’ in the model that allows you to pick just four or five surfaces to define the boundry, but those surfaces belong with the region you are copying. In order to include them, I’d have to pick a different set in the complex area (maybe 150 surfaces instead of 5, which is impractical). Sure I can make a second extract for those 5 boundry surfaces, then sew, but it would be nice to have the option to include the boundry surfaces in the extracted region or not, since I’ve already gone to the trouble to pick them. Additionally, it would be nice to have the option of adding or removing a couple other surfaces manually. The ProE equivalent that I am accustomed to used seed/boundary just as a selection method during the surface copy.

Again, until I see some sort of example it's hard to comment. However, there are some places where we use Regions where the Seed Face and Boundary Faces are NOT on the same 'side' as it were, such as Delete Face in teh Direct Modeling tools. So until I some examples it's hard to speculate as to whether there would be any advantage or not.

12) How do you specify a different draft angle for each side of a selected edge?

I assume that you're talking about when you're creating an extrude feature and using the draft option. Well once you have the preview on the screen, go to the Draft section of the dialog and in select the Draft option 'From Section' and then select the 'Angle Option' of 'Multiple'. Now you will have the option to define a different draft angle for each segment of the extrude profile.

No, I’m using the draft feature on imported geometry (mostly) with the ‘from edges’ type. It will draft both cavity and core side at the same angle, but I need to input different angles for each side. In some cases I have been able to work around by being sneaky with my edge selection to eliminate faces on one side, then apply a second draft feature.

OK, with the Draft feature we use a concept called 'sets', similar to Edge Blend where you wish to place a different radius on different edges, yet do it as a single feature.

What you do with Draft is select all of the edges that you wish to apply the same angle to and then select the little Green 'Add New Set' button and then select the next set of edges that we all have the same angle. You can go and assign a different angle to each 'set' of edges.


Well maybe that clears up a few items.







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/

 

[NXMold]

Thanks for the tips, this is really helpful information both on a specific and general levels.

6) Good tip!
8) I somehow missed that dialog, very nice to know!

10) See attached pic. This isn't the best example, but its one I have handy. I'm extracting a region that includes the outter (upper right) scalloped surfaces while the inner surfaces (bottom left) need to be excluded, the adjacent vertical walls need to be included in the region (marked 'boundary' in pic).

The vertical walls provide an easy to pick boundary, but then are excluded from the region and need to be extracted in a separate feature by selecting them all over again one-by-one, and then sewing, and living with a long feature list.

The only way to make it work now would be to pick each of the internal surfaces as my boundary instead, which is next to impossible (I tried!). If I could choose to include my boundary surfaces in the region then the vertical portion of the rib would be taken along for the ride, no extra picks and clicks, no cluttered tree.

I lived with this in ProE for many years, I came across it very often, but with proe since seed/boundary was just a selection method I could continue with manual selection and re-pick all the boundary surfaces a second time, all in the same feature. I still had to pick twice which was irritating, but now I have additional steps yet.

12) What happens is that I have, for example, a flat planar surface paralell with the Z axis that has been split or divided somewhere in the middle. When picking that middle edge for draft, both the upper and lower halves of the surface get drafted at the same angle. Adjacent surfaces further along the edge are not the concern.

 

[JohnRBaker]

For your extract region problem, have you tried to use the Region Option of 'Use Tangent Edge Angle' and select different angles and see what sort of result you get? Note that when using this method you don't have to pick any boundary faces just a single seed, but try it by picking one of your current Boundary faces as a Seed face.


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/

 

[NXMold]

Here's a fabricated example (see pic). In this case a single planar surface defines the boundary, but in order to include that surface in the region you can see that I'd have to pick 11 boundaries instead of one.

In most cases of course its not quite THAT obvious or simple, but I've been running into this for years.

 

[NXPERSON]

NXMOLD

Based on what you asked in statement number 4, you must be using a dual monitor setup. I have a laptop connected to a docking station which has a 19” monitor attached to it. I run my NX session on the 2nd monitor. This now leads to your response number 5. I to have tool bars docked vertically along the edge of the work window. Periodically, if I move the mouse before I release a mouse button a toolbar moves to a new row like what you show in your 5a.gif image.

When I have NX opened on the second monitor I cannot place the stray menu back in line. To realign the menus, I move the session of NX to monitor 1. Now I am able to realign the tool bars back inline. I then can move my session back to monitor 2. Maybe if a toggle button in the tool bar options was created to provide a lock/unlock toggle, it may reduce users frustration with this type of issue.

I have seen a related issue also when creating JPeG files from the Visualization tool bar. If the NX session is on monitor 2, NX fails to create the JPeG files. As soon as I move the NX session to monitor 1, NX then creates JPeG files without any problems. We are currently using NX4.0.4.2.

NxPerson

 

[NXMold]

YES! I'm also unable to print shaded images, and I do run on the secondary monitor. I'll have to check this out first thing monday morning, I bet you just solved at least two of my problems.

 

[hudson888]

John,

Thanks for your response about the use of layers or not. Funnily enough I have been working on a little side project that has obviously all been done on a single layer. The models are all very simple so I'm managing okay.

When it comes to the majority of the more complex models that we have worked on, class selection isn't going to cut it I'm afraid. Some of our colleagues love to model using a "chunky solids" technique based trimming primitives with planes, then uniting or subtracting, followed by blending and hollowing right at the end. It works well insofar as the geometry is remarkably light for the complexity of what can be achieved. the problem is they use a curve plane for each trim, and save them by the hundreds all on a single layer, (due to a misinterpreted corporate standard). Then there are the curves sheets and other entities bundled into, you guessed it, the same layer with everything else except the solid. Nobody can tell what's what with that.

So what I want to be able to do is collect groups of these objects according to their purpose rather than their entity type. First I extruded something then I trimmed it to three planes and a surface. Then I built another element from this extrusion and those trims... and so it goes.

Two ways I can see that you'd manage it. At the moment we use layers that's the first way. Perhaps we could manage groups in almost exactly the same way and we'd be able to do the same thing quite comfortably.

I wonder if you did something that shifted all the layer contents into group contents automatically starting at "NX-?" then added some dedicated group filtering to your show hide function then maybe that would be a way forwards.

I'm thinking in terms of having an infinite number of groups to replace a finite number of layers as a good thing. On the other hand I'm also thinking there would need to be virtually equivalent tools.

For the moment I suppose you'll struggle to get rid of layers simply for reasons of backwards compatibility. Mainly because the legacy of visible in view based on layers in drawings for example might be tricky to duplicate were you to remove layers entirely.

One thing that I struggled with at the outset is replacing many layers by using hide and show, because I equate that perhaps wrongly with only two layers. Yet by using layers there are four states Work, Visible, Selectable, Invisible. I'm with you so far as in reality there are only two states that matter either you can see it and therefore select it or you can't. You could get rid of work versus non work if you like, but if you wanted to work in the context of a category expressed say as the collected members of a group then maybe you ought to be able to. Think of it as similar to working in a sketch in that it collects a group of things with common purpose. I see the need to include categories or groups of objects that collect all sorts of things with common purposes together, so I'd like to see the tools to do that. At the moment what is available are groups managed by a same dialog that we've had for almost ever, whereas even layers have their own icons.

I'm happy to lose the layers as soon as they're replaced by something better, and I'd like to have a better way to manage how groups of dissimilar objects can be collected according to their purpose. I don't care much what it is called or whether it presents as a cunning new form of layer management that is done in whole new way using a replacement. The conditions I would place on it are the ability to collect dissimilar objects, and no work or additional cost required to shift over from the old system to the new.

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

Don't worry, as you've already commented on, it's going to be a long time before we could get rid of Layers even if we were trying to do that, which we are not, just that we're working on more modern and easier to use alternatives.

As I've mentioned the new NX 5 'Show and Hide' tool helps manage the visibilty of classes of objects. Also as mentioned we're enhancing the use of 'Remove Component from View' to make it easier and more effective. Also the the NX 4 behavior of where we can imbed a Sketch into the feature created with the sketch so that the display of and access to the sketch is handled automatically as part of the editing of the feature. Also inside of Sketches we allow you to create Groups that can collect different Sketch objects and then act on them as members of a group including visibilty, assigning color and so on. Now this was necessary due to the fact that by design, all sketch objects of any one sketch must all be on the same layer (that wasn't always true, and it was total chaos). But we've also added a similar scheme inside the Assembly Navigator where you can create Component Groups, again, you can control the visibilty by toggeling ON or OFF these groups.




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]

Thanks John,

And don't worry I wasn't really concerned that you wanted to get rid of layers. I didn't set out to mount an argument against anything you wrote, to "Save the layers". I just was intrigued to explore alternatives that might make managing the data easier within a file. It was the first time I'd given the prospect much thought.

In the end I had only one sticking point. I wanted to put the case for curves and sheets etc to be included among the new solutions that you're planning. They are an unavoidable part of what we do, and they're already seeming like the forgotten poor cousins of sketches and solids. Which is a pity because for much of our work we could get a result without using sketches, and many still do, but surfaces and curves in 3D space are irreplaceable. They're what sets Unigraphics head and shoulders above the majority, if not all of the other CAD systems.

Best Regards

Hudson

 

[NXMold]

I agree, I'm using a fair amount of curves sheet bodies as construction features and hiding them using a selection filter.

In ProE I had automatic layers setup that would 'catch' dautm planes, axis, points, surfaces, and curves. This way I could turn All_Curves off to cleanup the display. Curves could also be added to other layers to further refine the display. ProE layers were very advanced and useful.

 

[NXMold]

When I have NX opened on the second monitor I cannot place the stray menu back in line. To realign the menus, I move the session of NX to monitor 1. Now I am able to realign the tool bars back inline. I then can move my session back to monitor 2. Maybe if a toggle button in the tool bar options was created to provide a lock/unlock toggle, it may reduce users frustration with this type of issue.

I have seen a related issue also when creating JPeG files from the Visualization tool bar. If the NX session is on monitor 2, NX fails to create the JPeG files. As soon as I move the NX session to monitor 1, NX then creates JPeG files without any problems. We are currently using NX4.0.4.2.

Yup thats it all right, I can stack toolbars in a column on monitor 1 but not on 2. I also cannot print a shaded image from monitor 2, but it works fine on 1. Using 5.0.2.2