Full round and sketch references

[NXMold]

Couple of questions, maybe there is some lurking functionality that I haven't yet found.

1) Is there a way to view/list all external references in a sketch? This becomes most useful when trying to re-order features only to discover that a dependancy between sketches prevents it. The sketch needs to be edited to remove the errant reference, but currently I cannot find a easy way to search or manage these references.

2) How do I make a full round? I want a fillet that is tangent to three sides (one is consumed, the other two are usually paralell or less than 30° incl.). Some programs select the pair of edges, some the intermediate face. I suspect this may be possible in the Face Blend dialog?

3) It would be neat to have a custom toolbar with the last 5 used commands. Sometimes I dig way down into the menus for something unusual, then use it a dozen times in a row.

 

[cowski]

If you right click on the sketch in the part navigator and select "information" it will list the parents (objects the sketch depends on) and the children (objects that depend on the sketch) near the bottom of the info window.

Also, if you select the sketch in the list - the parents will highlight in one color (magenta on my machine) and the children will highlight in another color (blue for me). The first method is useful if you have a large navigation list and/or a lot of dependencies for the feature you are looking at.

BTW, this works for all features, not just sketches.

 

[JohnRBaker]

1) Is there a way to view/list all external references in a sketch?

If the objects being referenced are features (that is they show in the Part Navigator) then you can use the Part Navigator to show these dependencies. Just go into 'Time Stamp' mode and select the sketch of interest and all of the other items which are referenced by the sketch will turn Red.

2) How do I make a full round?

There is no direct function to do that but you can use Face Blend, if the conditions are correct, with limited success. Note that it's limited to only certain options but there is a very short bit documentation (on the 'How to' page) covering Face Blend. Generally I've had better success you swept surfaces and then either trimming or patching the final model to get what is a usable 3-face 'blend'.

3) It would be neat to have a custom toolbar with the last 5 used commands.

Well for NX 6 we are doing something very similar to this, but not at the Toolbar level, but rather with dialogs that have long lists of options. The user will have the choice to either continue to use these lists of options as they do in NX 5 or they can ask that the list be presented as a set of small icons in the dialog and then if there are more options than there is room to display all of the options, the icons shown will continue to update based on your usage, so like your idea, the last used will always to immediately available to the user. Attached below is an image of the same dialog (in this case, Assembly Constraints) shown twice, first with the drop down list as you might see it in NX 5, but with 'Show Shortcuts' option added, which if you select it, it will then present the Constraint options as a series of 6 icons representing the recently used methods. And if you discover that you need something different, you can still pop up the list and select the desired method which will of course then replace one of the 6 items in the series of Icons. Note that both the Icons shown and the fact that you using the icons instead of the list if options will be saved by Dialog Memory so that once you set these they will remain in place until you either reset the dialog or choose to go back to a drop-down list.


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]

Good info. Too bad about full rounds, its a handy bit of functionality when you need it and helps to prevent over-constraint.

I need to clarify the sketch issue, suppose you have sketch #1 with an extrude and boolean, then sketch #2, extrude, boolean.

Extrude #1 is a parent to sketch #2 (as seen in red/blue in the feature tree) because there is a geometric constraint in sketch #2, perhaps a tangency. This tangency constraint could very well be made to another piece of geometry instead, and indeed should be. The order of the sketches needs to be reversed, the dependency in this case should never have been created, but as complex as some sketches are it is difficult to find the constraint (on edge, tangent, equal length, a dimension...) to delete it.

It would be nice if there was a reference manager (like proe) where all referenced geometry external to the sketch was listed, and could be manipulated.

This way I could list references in sketch #2, see edge of extrude #1 and delete it. My sketch would no longer be tied to the earlier features, and I could re-create the tangency constraint to the proper edge.

 

[hudson888]

What you have is the kernel of a good idea and some basic criticisms of common modeling errors. Inasmuch as problems of people modeling themselves into corners may be possible even frequent and often inadvertent I would be the first to agree that managing where associativity occurs so that it can be decoupled and re-applied as required would be a good idea. And by extension some visibility of the various associative elements would be a requirement of that.

On the other hand your discussion centers around the idea of sketched based extrusions where the problem becomes that in some part the sketches reference one another. Since it may also be possible to constrain elements of later features and/or sketches relative to edges of the first extrude for example then you have even more possibilities to analyze before you are able to quantify all associative aspects of the model. In recognizing that circumstance you may have to concede that as complexity increases so does the burden of analysis.

Ultimately I would rather forgo associativity on the odd occasion than give up the flexibility of having the option to apply it as needs see fit. What we are talking about in effect often evolves around changing the design such that original assumptions as expressed by associativity may no longer apply. Depending on the scope of the change you may even do better to simply start again.

For the moment you will find that although you may prefer to use sketches NX is a fully flexible system that provides many solutions to such problems that are often easily applied by going beyond the sketcher. While on one hand you may rightly argue that it adds complexity to offset, replace or delete a face rather than manipulating the original sketch the principle involved is that if the system provides the flexibility to achieve results without exhaustive analysis then that may offer better "bang for your buck", (in the NASA sense of the term not the Governor of New York ).

Best Regards

Hudson

 

[JohnRBaker]

It will be interesting to hear these same topics discussed after NX 6 is released (or at least launched) since I suspect that many of you will perhaps have to rethink what is and what is not a feature-based model or how changing details of a model will impact the rest of it. I'll leave that teaser with you for now and just suggest that you keep your eyes and ears open for when we start the NX 6 launch in April and if you're invited to an 'event' in your area that you seriously consider participating.


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/