Items UG needs to fix!! 6

[HellBent]

I just posted in another thread how I'm always telling myself I need to write down the minor "annoyances" I have to deal with everyday while running UG but I just never seem to do it. For some reason I think having a thread dedicated to just that may help. At some point maybe these items will get the attention they deserve by UG. So I'll start it off with a couple that immediately come to mind:

#1. Fix the darn 2d translators!! Why does making a DXF or a DWG of my drawing have to be so difficult? It has never worked right! Why am I forced to run it through CGM in order to get reliable results?

#2. Let me fix errors during feature creation rather than having to start all over again. I.E. "Through curve mesh" intersection errors force me to fix the intersections and then start all over again. Let me edit the intersections from within the creation menu so I don't have to re-select all of my geometry again! Apply this mentality to all feature creation...give me the ability to fix mistakes on-the-fly.


I think I'll be more likely to add items to a thread on a message board than write them down on a notepad so let's give it a shot!

Take care...

 

[Agriego]

Is there a way to convert a detailed thread feature to a symbolic thread?

Sorry, but no. At the moment they are created as two different types of features.

I was afraid of that. I was hoping to avoid deleting the old thread and recreating it, but it's not a big deal. The pain is to have to create seperate sized parents for my fastener part families. It would be nice to be able to have a field where I can call out the threadform I want in the part family spreadsheet.

Thanks for your help. It's great to be able to post a note and get answers straight from the source.

Al

 

[JohnRBaker]

What I've done in situations like that is to create both a symbolic and detailed thread feature and then use Suppress by Expression and just set up a single expression value so that when you change it, so from a 0 to 1, it will suppress one feature and unsuppress the other.


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

http://www.siemens.com/plm

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

 

[man2007]

John,

Ug will not allow putting rectangular window or 'window selection' while CREATING the blend, I tried it.

Even I tried to select the EDGES FIRST by
1) Setting the selection mode to 'general objects' (By hitting 'G' key)
2) Then put a rectangle to select the edges
and right click on the edges->select Blend... option, but unfortunately ug deselects the edges I selected and will prompt me to select new ones. For single letter like 'N' (which doesn't have smooth edges like in 'S' or 'O') also this method fails.

-man2007

 

[JohnRBaker]

Man2007,

What version are you running? I assumed you were running NX 5. Sorry, but in NX 5, you can area select when creating Edge Blends.


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

http://www.siemens.com/plm

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

 

[man2007]

I had mentioned it earlier, it is NX 4.0.3.3.

-man2007

 

[hudson888]

When it comes to some of the selection issues you have mentioned I see that there are arguments on both sides and I won't bore you by taking that issue any further. What I did do however was to work through a couple of examples that guys have mentioned here most recently in this very long and meandering topic.

Here are some thoughts.

It's about time you could pick more than one boundary within a general pad feature. The letters A,B,P,R in capitals are all impossible. Why not make it that whole words could be done.

When blending, or tapering anything with a great number of edges to select then one of the best selection tools available is to use "Select all edges in face". It is just a damn pity that it is implemented as an all or nothing option. Many times the face has central edges that you want to apply blends to and yet it would be either impossible or undesirable to get the same blend/taper to work on the boundary edges or some smooth edges of a sewn trimming surface earlier applied. What needs to happen in that case is that you make then initial section using all off face thereby including the overwhelming majority of edges that you need to select, but you are then able to deselect individually the fewer edges that you need to exclude. Currently no matter how I try to do this it doesn't work. I'm certain it would be a valuable enhancement and it may provide the work around that previous posters to this topic are looking for.

Under some other dialogs where window selection is available the same all or nothing behavior occurs. I was thinking of curve projection. You can't shift deselect those one or two background objects that got inadvertently included in the selection window. It is annoying and I think not good enough.

In earlier versions of UG to control how selection confirmation works you could hold down one or two extra keys to turn it on or off. This was really good I still miss it. Why can't you please re-introduce that or something like that. The current situation is that you have either to confirm everything or set a delay and then wait, neither is nearly as good as being able to exert my control over the ability to use it when I need to.

I have been working mainly in NX-3 and tested in NX-4. We have NX-5 but not to work with for long enough to comment with any certainty yet. Therefore it is possible that some of the solutions I have alluded to may have been implemented without my knowledge.

Best Regards

Hudson

 

[JohnRBaker]

In earlier versions of UG to control how selection confirmation works you could hold down one or two extra keys to turn it on or off. This was really good I still miss it. Why can't you please re-introduce that or something like that. The current situation is that you have either to confirm everything or set a delay and then wait, neither is nearly as good as being able to exert my control over the ability to use it when I need to.

OK, try this. The way I've got my selection set up is that under Perferences -> Selection... under 'Highlight' I have 'Highlight Selection on Rollover' toggled ON and the delay set to '3'. However, under 'QuickPick' I have that toggled OFF. Yes, OFF.

Now this may seem odd, particularly since, as you've pointed out, we've removed triggering Confirm using special second keys. However, you can now basically use QuickPick like you've done in the past since now when you place your cursor over some area where there are multiple objects that could be selected, while the first item will highlight, no matter how long you wait, the 3 periods (...) will NOT come up so it never gets in the way of normal picking. However, if you wish to use QuickPick (i.e. 'Confirm') just hold down MB1 (left mouse button) for approaximately 1/2 second and the 3 periods will come up and you can then go directly into QucikPick as normal, just without having to either wait or having to use a special second key.

Anyway, try it, I think you'll like it. I know I do.


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

http://www.siemens.com/plm

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

 

[hudson888]

Thanks John,

This sounds like just the thing I need to be doing.
Under which version are you describing it?
In NX-3 I have pre-selection turned on, and have now reduced the delay to 3, from something that was much higher, probably too high. I'll try it like that for a while, and I'll look into settings for NX-4 also, we're still really waiting for NX-5 so if that has been improved I'm keen to see it for myself and pass on my congratulations if indeed there are some real improvements.

The remainder of my earlier comments were substantially exploring the idea that my tinkering lead to, which was about how the requested "thing to fix", could be addressed in a few different ways.

Best Regards

Hudson

 

[JohnRBaker]

For NX 3 I would set the Preselection delay to 20 (Preview Selection in NX 4) as that's a 0-100 range scale.

However, in NX 5 this has been changed to six descreate settings, displayed as 0 to 5, so a 3 in NX 5 is NOT the same as a 3 in NX 3 or NX 4.


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

http://www.siemens.com/plm

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

 

[Crocostimpy]

Good stuff, but back to the original thread intent. I was a ProE user for 12 years, so a lot of my complaints are born out of just being used to something else. But two of my biggest complaints are:

1. Why oh why can't helical curves be associative? I design bottles. Every one of them has threads on it. If I change the heighth of the bottle after adding a thread, the thread goes kaput. Actually, the way I create them, the thread will tolerate small changes, like say .060" or so, but anything more and the sweep won't follow the curve. I have to delete the thread and all associated features, including the helical curve, and create them all over again. I thought this was a parametric software.

2. Why can't hidden lines be easier to deal with in Drafting? If the hidden line becomes solid as it comes around the model, then the solid line gets erased too. I've tried splitting the lines but that's too labor intensive. I don't even bother with hidden lines anymore.

This is on NX4, although I've used NX5 at a previous employer and had the same problems.

Mike

 

[hudson888]

Mike,

You make points both of which are valid in terms of you intent to use the software in a certain way. It may be possible that future enhancements will come along to address some of your concerns. I hope that people who post here are often heard by PLMS, but you could of course put in an ER as well.

You also mentioned about users who come in with a different approach based on their use of other CAD systems. In the same way perhaps I would approach your task differently mindful of the limitations of the system as it stands. They may still be limitations that you don't much like, but there's nothing wrong with trying to make your life a little easier.

For the bottle threads, you could design the bottle with the datums near the thread rather than the base so that upon updating the thread end always remained intact. Another way would be to create your thread in a separate model mate that to the neck, wave link the thread portion and unite that to the bottom of the bottle solid.

For the hidden lines, while I agree that they aren't easy and could perhaps be better I would have to say that I have so little call to manually edit them that it really doesn't bother me. I wonder how and why it comes to be that you have to manually edit hidden lines frequently enough that it becomes a problem. If you want to start a thread describing exactly what you're doing and how, then we may be able to give you a few pointers towards decreasing your suffering to tolerable levels.

Best Regards

Hudson

 

[phillpd]

Mike, try using a Law Curve (to drive a helix) rather than the Helix Curve, you'll get the same result BUT the Law Curve can be parametrically positioned.

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[Crocostimpy]

I've been playing with the method outlined by John Baker in thread thread561-164528 using a law curve to make a helix curve. It works great as far as being able to move the helix curve around, or the helix curve moving as the height of the bottle changes.

The problem comes after I make the Swept thread feature. As soon as I move the curve, or it moves as a result of another change, the sketched curve defining the thread flips upside-down. The curve is sketched on a plane created at the end of and normal to the helix curve. I'm not sure what's actually happening here; if the normal direction of the plane is flipping or if it's because of the way my sketch is constrained. Or maybe something's changing in the initial surface created to define the helix.

Incidentally, I'm making the thread as a Swept feature because when I make it with a Sweep Along Guide the thread profile twists somewhat as it follows the guide. Using Swept I can select Face Normals, select the face of the revolve that the thread is going to sit on, and the shape doesn't twist.

Any suggestions for what I might be doing wrong are appreciated.


Mike

 

[Crocostimpy]

Ok, I need to clarify this a little. When the sketch flips it flips upside-down but also becomes aligned with the end of the helix curve, not the start end anymore. The plane it is sketched on remains relative to the start.

And to make matters worse, when I make the helix curve something other than a full turn the sketch really gets screwed up. I think I definitely need to look at how I'm constraining the sketch for the thread.

Any jabs still appreciated though. ; )

Mike

 

[JohnRBaker]

Mike,

Could mail me the part file?


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]

Mike,

I'd say that what you have done is used the helix curve to create the plane one which you have then sketched the thread profile. When the helix moves then the plane moves, but because the plane is loosely anchored only to the curve then there is no vertical or horizontal directional vector anchoring your sketch. You may find that you can create a datum axis that you use to set up you sketch plane using two points taken from the helix construction geometry. You'll find these datum axes to be associative enough and even if the axis does not lie on the sketch plane it should still work.

Two obvious choices are that if a helix axis exists then the end of that and the adjacent endpoint of the helix might do he trick. Otherwise if you always use a round number of turns in your thread then the two ends of the helix might provide a useful construct for a datum axis. Even the axis of the helix itself as a curve could provide the basis for a datum axis that will keep your sketch facing the right way up.

If you don't have geometry that you know of with which to do this then you may have to create something perhaps as part of one of the other sketches in your model.

One other factor to consider in this is the shape of the thread form. There are several possibilities whereby your threads may be modeled without a sketch and that would also make the problem go away. For example if it is essentially a circular profile then use a tube rather than sweeping anything. I had an example of this with a fellow mid last year. It was great practice for me to brush up on my sweeping knowledge in explaining all about it to him, but at the end of the day it turned out to be a simple circular profile best done with a tube.

A lot of other profiles can be created starting with just a line which you would probably have to sketch so it follows the helix up and down as the bottle height varies. But if you sweep a line you get a sheet, which can be thickened, tapered, blended as required to arrive at a thread form that having been built in this way should be less likely flip over when the model changes.

And if all that still won't work then as I said earlier it would be easier if you modeled the bottle from the neck down, rather than the base up. Some of these problems would be alleviated.

Regards

Hudson

 

[realmagicracer]

1) Perhaps it's necessary to make easier way to set dimension standards.
For example - to change the view of dimension line and then to set it as default in "Customer defaults".
2) To keep the drawing standard settings not into prt-template file, but in settings file (Customer defaults). So it would be easier to change the default settings in the templates without creating new template file.

Regards: Dimo Urumov

 

[Crocostimpy]

John, I've been playing with it and have gotten it to work pretty good. The key was not to align my sketch to the end of the helical curve. Something was causing it to go wonky when I did that. Once I inserted a datum point, not associated with the helical curve, and aligned the sketch to that point, it started working pretty good. I don't have the version that I was having trouble with anymore, but I can recreate it if you're still interested in seeing it. Let me know.

Hudson, as I said above, I've got it working pretty well. It turns out the sketching plane wasn't the problem but the way I had the sketch constrained. At least that's the way it looks so far. The shape of the thread profile is such that I think it is easier to sketch it. Or maybe that's just me. Thanks for your tips.


Mike

 

[JohnRBaker]

1) Perhaps it's necessary to make easier way to set dimension standards.

In NX 5 Customer Defaults, we have now implemented a 'One Button' option to select a predefined 'Drafting Standard' as an alternative to setting a bunch of individual items. The included default Drafting Standards (yet still customizable) are ASME Y14.5M - 1994 (which can also be set to comply with either the ANSI Y14.5 - 1982 or the GM Addendum to ASME Y14.5M - 2004 standards), ISO 1101 - 1983, DIN and JIS.

2) To keep the drawing standard settings not into prt-template file, but in settings file (Customer defaults).

Also for NX 5, we've added on option in Customer Defaults so that when using an existing Drafting Template, that the system either honors the drafting setting in the Template Files, or it OVERRIDES those settings and uses the explicit Drafting Standard selected (as discussed above) in Customer Defaults.


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]

Mike,

As long as it works .

The ability to do things so many ways is the beauty of UG. That alone made me confident we could always find you a way out.

Regards

Hudson