Sketch convenience options 2

[PrintScaffold]

Greetings all!

I have two minor questions regarding convenience of work with the sketch in NX8.5, I thought it is ok to put them both into one topic.

1. When the sketch is on the layer other than work layer, NX switches to that layer when I start sketch task environment. But it does not do that when I start sketch edit directly, making me manually switch the layers. Is it possible to automatically switch the layer when using direct sketch edit?

2. When direct skectch edit is active, I see skecth X and Y axis, and also a sketch plane. Is it possible to make this this plane permanetly invisible? It's really unneeded for the task.

 

[JohnRBaker]

First off, why are you placing your sketches on anything other than the Work layer? Are you going to use these sketches to create features using tools such as Extrude or Revolve?

As for your second question, NO. These items are always displayed when a sketch is opened since they are, by definition, PART of the Sketch (they contain referencable datum objects such as a point, axis and plane).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

Hi John!

Question #1. Yes, I always put sketch on one layers(s) resulting solid/sheet geometry on another. That's why I find it inconvenient to face the need to manually switch to the layer where the sketch is located if I need to edit it.

Question #2. I can't see the need for the plane. Am I missing something?

 

[JohnRBaker]

Until you have more than one or two curves in your sketch it helps to show the plane of the sketch. This is particularly helpful if you're working with the Direct Sketch in an orientation which is NOT parallel to your current view. Please note that starting with NX 8.5 we've at least dumped the 'Z-Axis' since this was totally useless when working in the 2D space of a Sketch.

As for the layer issue, the intended AND recommended (and out-of-the-box default) workflow is to allow the sketches to be imbedded/absorbed into the modeling feature as this will automatically 'manage' their visibility (to say nothing of decluttering the Part Navigator). Whenever you need to gain access to the Sketch it will automatically be available when editing the modeling feature and besides, you can now gain access to the Sketch dimensions from the screen, without even entering the sketcher, whenever you edit a modeling feature which contains an imbedded sketch. Also, if you wish to reuse any of the sketch dimensions as PMI objects, if you're using layers to manage the visibility of the sketch you will be making the PMI object invisible as well. However, if you allow the system to manage the sketch for you by imbedding it into the modeling features, the PMI objects will remain visible even when the sketch itself is removed from the display.

If you just allow the system to work as designed, I think you will see that you will be spending less time performing 'bookkeeping' tasks and you will not have worry about where and how to get access to your sketches. They will be there when you need them and out-of-sight (and mind) when they are not.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

I never heard before that NX is designed to be worked with automatic embedding of sketches into the feature. First of all, sketches are not automatically made internal when features are created. Second, one sketch often is used for multiple features, and that is the most efficient workflow in many cases, particulatily when free-form is concerned, or when we design a complex control structure for a big assembly. How about that?

 

[capnhook]

PrintScaffold, you just have to get used to "hiding" everything everywhere. Remember when you were a kid, and someone told you to clean up your bedroom? You hid everything you didn't want anyone to see under the bed, in your closet, in your brother's closet, etc. Pretty soon you had a nice clean looking room.

Same thing in NX. Hide the stuff you don't want anyone to see, and then you can pass your work off to someone that might discover all you have hidden at a later date. Let them worry about not knowing what is junk, and what is really needed. If they throw away important stuff, then that is their problem.

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[JohnRBaker]

Traditionally UG/NX never attempt or even offered an option to automatically, or for that matter manually, imbed Sketches into their modeling features. However, this all changed when we started to transition Ideas users over to NX as not having this as even an option was a big deal for them as that's the way they were used to a CAD system working (which was also the case with many other CAD systems which used 'sketched' profiles when creating modeling features). Our initial reaction was exactly what you said, "But a sketch might be used to create more than one feature so how would that work?" And to prove our point we looked at literally hundreds, is not thousands of the parts which had been sent to us over the years from customer either when reporting problems or when we specifically asked for real-world examples for our internal regression testing. Well, the results were quite illuminating as it turned out that something like only 3% or 4% percent of all sketches were ever used to create more than one feature. Sort of undermined our long-held position that this was something that we didn't think would be very useful, that is automatically imbedding sketches into their modeling features. So we changed our mind and went forward with this new and more modern workflow, however we did make sure that this was BOTH an optional behavior (it can be disabled in Customer Defaults and/or Modeling Preferences) and that it would be easy to make 'external' a sketch which was originally created as an imbedded item (and vice versa so that existing models could be 'cleaned-up' as it were).

And once we got into this mind set, we started to take advantage of this 'automatic' management of sketches with things like allowing you to access sketch dimensions while in the feature edit mode as well as the previously mentioned PMI support, both of which would be hindered if you choose to 'manage' your sketches manually using Layers or Show/Hide.

Now don't get me wrong, if you want to work the way you described, there's nothing stopping you because if nothing else, NX has ALWAYS supported multiple ways to do most everything ever since I can remember, and come this August, it'll be 36 years since I sat down in front of UG 'workstation' for the first time.

Besides, the title you chose for this thread, "Sketch convenience options", sort of indicated to me that you were looking for the most "convenient" way to use sketches in NX. However, having to 'manage' them yourself and accepting the less than ideal behavior that you may then run into later could hardly be seen as making sketching more "convenient" now would it? But as I said, if we didn't think you might want to do things differently, we wouldn't have made all of this optional. We could have just coded it to work in one manner only and left it at that.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

Thirty-six years? Wow! Come this August, I'll be only 35 years old.

Still, if we look at any software product old enough (matter of decades), we will see that a lot of features which were introduced over time are disunited and implemented inconsistently. This absolutely applies to the sketch editing behaviour, resulting in layer switching in one case, and not switching in another.

I will try working with sketches as you suggest as I always open to new ideas, especially ones promising to improve productivity. But the one sketch/one feature approach is still limied to the piece parts in a bottom-up workflow. When we look at the top-down workflows, for the creation of a control structure the only approach worth talking about is creation of few complex sketches representing all key features of a product. Doing it otherwise defeats the very idea of a control structure.

Bottom line is that it would be nice to have layers switching after activation of sketch for direct edit.

 

[CADMANSOUTH]

To hid the sketch planes in NX6.
Put the planes that the sketch uses on a different layer then the sketch. In this case the planes/axis/Datum Coordinate System is a separate feature from the sketch.

For example planes on layer 31 sketch on layer 21.
Turn on the layer 31. Edit the sketch. Turn off layer 31.

If you do not turn on layer 31 before editing the sketch the planes will be temporally moved to layer 21 untill the sketch edit is done.

 

[JohnRBaker]

I don't think PrintScaffold was referring to a Datum plane which may or may not get created when you start a new sketch, but rather the 'plane' object which is part of the so-called CSYS of the Sketch itself...

...which can be temporarily Hidden while working in the Sketch but which will always be displayed when the Sketch is reopened in the future.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

John, I tried working to your advice, and immediately became stuck. How do I edit a sketch when it is embedded?

 

[JohnRBaker]

Well there are several options depending on what exactly you're attempting to edit.

If all you wish to do is edit the Constraint dimensions that you added to the sketch (NOT the so-called 'auto-dims') you have two options. 1) Select the Feature with the imbedded sketch in the Part Navigator, expand the 'Details' panel at the bottom of the Navigator and edit the dimensions from the list presented. 2) Double-click the Feature on the screen and when the Sketch dimensions appear simply select the desired dimension and edit it.

Now if you wish to edit something other than just the existing Sketch dimensions, such as a Geometric Constraint, or you wish to add or remove Sketch curves, you also have two basic options. 1) After double-clicking the Feature of interest, when the Feature edit dialog is displayed, in the section of the dialog labeled 'Section', select the second icon from the right labeled 'Sketch Section'. This will cause the imbedded Sketch to made visible and you will be taken into the Sketch editor where you can perform any sort of edit that you wish. After editing the Sketch when you hit the 'Finish Sketch' button, the editor will close the Sketch will be automatically re-embedded. 2) You can always un-imbed the Sketch by going to the Part Navigator, selecting the feature of interest, press MB3 and select the 'Make Sketch External' option. Now the sketch is it's own standalone feature and can be edited as if it had never been imbedded in the first place. Note that after editing the Sketch, as long as it has not been referenced by more than one object, either a modeling feature or another Sketch, if you select the original feature of interest in the Part Navigator, press MB3 you can re-embed the Sketch by selecting the 'Make Sketch Internal' option.

Anyway, I hope that helps.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

Yes, it does! Thanks, John.