NX-5 New hole feature sketch problems 2

[hudson888]

I seem to be having problems with the new hole feature or at least the sketches thereof in NX-5.

I created a block with a rectangular pocket and four holes in the base of the pocket, and another hole off to the side that has nothing to do with the rectangular pocket or the other holes. The first four holes were made using the new hole feature. I allowed it to throw me into the sketcher where I created four points for the holes and added inferred dimensions from the corners of the rectangular pocket by picking it's near edges. The result was a rectangular pattern of counterbored holes from the rear of the rectangular pocket. The third hole was another counterbored hole from the same side of the block as the rectangular pock and positioned using another of these embedded sketches to the corners of the block. Everything appeared to be working well. I went on to create a mirrored set of these features and finished the model with the minimum of fuss.

Next day we decided to change the design slightly and that is when the fun started. The change required that the pocket be moved nearer to one end of the block. The third hole would follow it. I changed the positioning dimension for the rectangular pocket, which updated correctly, but to my surprise the four holes became three. When I checked the sketch embedded within the hole feature I found that two of the points were on top of each other, and one of the dimensions had been assigned an incorrect value. I corrected this and when I finished the sketch the holes went into another whacked out pattern two on the centerline and one either side thereof, but back to four holes. Again edited the sketch deleted all the dimensions this time and recreated them until it looked correct, hit finished and got yet another wrong pattern of four holes the opposite of the previous one.

I used undo back to the start and just tried to move the third unassociated hole. The model reevaluated the feature list counting down in the Cue status bar as it does, and guess what, but the pattern of four holes took another turn for the twilight zone. I tried separating the sketch to no avail etc etc... Basically I bashed my head against this brick wall of a thing and swore at for a bit until I realized it was a waste of time. .

In the end I deleted the new hole, used the old one with a rectangular array, and have no further problems.

I just want to know is there a problem with these new hole features, or sketches in NX-5.0.2.2, and if so has it been fixed in NX-5.0.3x or 4x, upcoming.
Otherwise is there something extra that I ought to do with the sketch to force it to behave in a more stable manner? In other words I obviously believe that I ought to be able to do exactly what I am doing and expect to get a reliable result, however if the system can't cope with that what more should I do to have it work correctly, or am I doing something wrong misunderstanding the capabilities of the sketcher in NX-5 or something?

I'm running NX-5.0.3.2, but at the site where I was modeling up some parts recently they're using NX-5.0.2.2. I mention this because for the first time we are seeing errors saying "feature created in a later version", so I suspect that the point releases aren't entirely compatible.

Any Clues

Hudson

 

[JohnRBaker]

Hudson,

Since your model sounds rather simple, could you create it up to the point where you tried to edit it, save it and attach it so that I can take a look at it?


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

http://www.siemens.com/plm

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

 

[hudson888]

Thanks John,

I'm off-site at present but will post it in the original as near as I can as soon as I am able.

Best Regards

Hudson

 

[hudson888]

John,

The file is attached as promised. I tried to recreate the problem using NX-5.0.3.2 as I described the construction technique above, and could not fault the model. I may have been over simplistic in my explanation, however with the attached model there is no longer any need for that conjecture.

I had my colleague e-mail me the file and have managed to copy it, remove some inconsequential features, and provide a copy that is both non-identifiable for the sake of any of the company's sensitivities yet demonstrably reproduces problems with the four counterbored holes. This I have also done in NX-5.0.3.2

Simply open the file and have a look at the way the hole feature for the four counterbored holes is dimensioned. Then change the positioning dimension for the rectangular pocket from -30 to +10. When I do this one of the holes repeatedly loses one of its sketched dimensions and ends up positioned in the wrong place.

All of the subsequent phenomena that I described in NX-5.0.2.2 were genuine although editing the single hole was not causing me problems in the attached file.

I had only posted in the first instance to prompt some sort of response along the lines of a known problem that could be fixed with one of the later patches. As it has turned out I suspect that if we can reproduce any such symptoms in NX-5.0.3.2 users other that John may not have any newer patches so I hope this helps illustrate and correct the problem.

I will take it as read that had I created the model as advertised in my original post I may have had less problems. However when I initially found the problem using NX-5.0.2.2 I did endeavour by editing the parameters of all the affected features to simplify the model such that it was separated from the other sketch. That sketch used elsewhere in the model (not shown in this version) seems in part to be necessary in reproducing the behavior that I'm having trouble with. However given that I could all but delete it after my initial attempts at remedying this to no avail I think it is not entirely to blame and that there must be more to it that my analysis been able to show.

I'd happily be shown up for doing something wrong in this model if that were the case, since I have been free and fast with the new hole feature and it would soothe our nerves to think it was not going to let us down in the manner too often.

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

OK, attached is a zip file containing 2 files. The first, XXX_jrb-1.prt, I just went in and cleaned-up one sketch dimension (it appears that you had selected some temporary curve that wasn't really the edge of the pocket). I also deleted and recreated the mirror feature. Now it works fine, at least in NX 5.0.4.1 (you should still be able to open this in NX 5.0.3.2).

The second model, XXX_jrb-2, I redid your sketch for the 4 holes just as a demo of how you can create simpler sketches with less dimensions and constraints. One thing to keep in mind when creating sketches for the new hole function. The only objects recognized by the hole function itself are the points. All other objects, while they may play a role in the sketch to help locate and constrain the points, mean nothing to the hole function and are therefore ignored. You don't even have to make then reference, they are ignored automatically. If you look at my second model you will see how this saved a bunch of redundant dimensions.

Anyway, take a look at what I've done.

And one other thing. If you're going to insist on working with long skinny models, please turn Perspective ON since it makes your models a lot easier to view and understand ;-)


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,

Thanks for your help I will indeed use your models as a guide to more reliable techniques for the time being, and I appreciate that you've taken the time to look into this for us.

I agree that it could have been better done because I did so later on, which is not to labor the point too much that the earlier version appeared to work until editing manifest some problems. I was very frustrated by it since the problems did not to my mind appear to be predictable based on the method first used. In other words in hindsight there is a safer way, but that would not infer that the method used shouldn't be expected to work. The way it was initially done expressed the design intent better it terms of the relationship with the other sketch, because it took dimensions as drawn from the mating part which was a purchased catalog item. Unfortunately what I found so far for myself was that once I separated the other sketch from the embedded sketch for the hole feature my problems seemed to clear up. It is behaving quite convincingly like the dimensions of the sketch are doing a poor job of keeping up with tracking which side of the centerline of the other sketch that they're applied.
The only point in all that is whether if it should have worked in the first instance there can be some remedy for this sought in NX-5.0.4x or beyond, but hopefully before NX-6.

Keep in mind that what I was able to reproduce in NX-5.0.3.2 is only half as bad as what I was getting in NX-5.0.2.2 during my initial struggles with this problem. Which unfortunately I won't be fully able to share with you at this late stage.

That reference line thing was something that I observed to have showed up when the problem occurred. However I can assure you that I did not create any such thing I have no idea where it came from and interpreted it as a symptom not a cause.

Anyway I hope this has been of some help, and again thank for your help .

BTW, yes the perspective helps. I was getting too much though and couldn't find where the setting had gone to allow me to change the viewing distance?

Best regards

Hudson+

 

[JohnRBaker]

Hudson,

The reference line problem was due to the fact that when you selected the edge of the pocket it had been split into TWO edges due to the placement first of the larger hole. Therefore one dimension got attached to one half of the edge and the other to the other half. After the update, there was only a single edge and one of the dims got 'lost'. I fixed it by doing the edit, then going into the sketch and fixing the one dimension and then changing the 10 back to -30 so that the pocket went back to it's original place, but now the dims were pointing to the same edge, by definition. If you had created the 4 smaller holes first and then the single larger one, you would have never had any problems either. Unfortunately these are the sorts of pathological things that you can't predict and which is very difficult for the software to accommodate.

Anyway, that issue has nothing to do with the New Hole function as it could effect any Sketch in general.

As for the perspective, I generally just do a Fit as that usually solves that issue, but if you want to really change the observer distance, now in NX 5 it's really easy as that's what the new 'Camera' option allows you to do.


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,

Didn't investigate the camera option my bad. No wonder the command finder didn't pick it.

Thanks for the edge explanation not only am I glad to know it is just the sketch pathology and not the hole feature as such, but I hadn't picked up why that went awry until I read your analysis. The hole splitting the edge makes two edges so that one no longer exists when the design changes, and therefore the dimension loses its reference.

I'm still somewhat of the persuasion that the degree that it was misbehaving in NX-5.0.2.2 was to do with the dimensions changing sides relative to the centerline of the other sketch and/or the pocket. This simply because the degree and number of different solutions that it threw up were out of control. As I said I'd edit the sketch until it looked right and was fully constrained and then when I exited the sketcher and updated the feature it did something that seemed unpredictable. This of itself kind of freaked me out so that I never analyzed the example that I gave you in the same logical manner. So while I'm both happy and in agreement with your logic I'm still unsettled about what was going on the other day in NX-5.0.2.2. I'll write it off as a bad day adopt more careful sketching practices and presumably it won't happen again.

Thanks again for you help. Shiny star and all that

Best Regards

Hudson

 

[JohnRBaker]

Hudson,

There is another 'pathological' issue with sketch's. Last year on another message board, I posted basically the following item:

What you've encountered is something that in the world of mathematics is referred to as 'Chirality'. In simple terms, what it means is that some shapes can't be changed by simply changing the parameters that define the locations of the points.

For a more detailed explanation, try going too:

http://en.wikipedia.org/wiki/Chirality_(mathematics)

This often occurs with 2D shapes that are being defined by a series of simultaneous equations that can be edited so that when they are solved, the shape changes (gee, this sounds amazingly like what many people call a "sketcher" ;-). Now one of the tricks that people have used is to 'sneak up' on the value that you're having a problem with. Now, I'm not a mathematician so I can't give you the exact reason why this works this way, but it has something to do with simultaneous equations being more robust if they're solved in a series of small steps rather then one big one where everything has to be resolved at once.

In the case of NX we have known of this 'issue' for several years and have made, and continue to make, tweaks to the way we solve these sorts of Sketcher equations so as to mitigate this 'Chiral' effect. Now I know we've made some recent improvements with NX 5 and I assume that we will continue as needed.

Anyway, I know that this sort of thing can look strange and is often frustrating, but these are the sorts of issue that we continue to invest time and effort addressing, often with little fanfare and even less glamor, yet we do it knowing that this is what contributes to having robust products which behave as expected.

I hope this helps explain some of the other behavior that you may have seen in the past, and may still in the future, just hopefully not as often.



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]

Who knew a simple sketch would lead me to expand my knowledge of Möbius strips and Klein Bottles.

http://en.wikipedia.org/wiki/Klein_bottle

I'm looking forward to seeing one of these beauties modeled up in NX sometime soon.

Thanks again John for the explanation. I thought was going nuts for a while there so I appreciate the fact that you took the time and also revealed a bit of the knowledge behind how it really works.

Best Regards

Hudson