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Sketches hidden in bodies

Sketches hidden in bodies

Sketches hidden in bodies

(OP)
thread561-244099: Sketch Visibility

This thread describes that sketches are invisible when created inside a body and that the only way to make them visible is to make the body transparent. This was NX6. In NX8 the problem persists. Is there a single good reason for hiding sketches inside a body? It is extremely irritating that when creating a sketch it disappears, leaving me in the dark as to whether it was created successfully or not and what it looks like. Then when making an extrude based on the sketch I have to click in the part navigator instead of the graphics view which is the more intuitive way.

RE: Sketches hidden in bodies

hi cnszu,
there are some settings from customers default controlling this behaviour. customers default -> search for internal...
hope it helps

RE: Sketches hidden in bodies

Were you aware that you can go to the Part Navigator, select a feature created using a sketch, press MB3 and select the 'Make Sketch External' option which will cause the sketch to now appear both in the list of features in the Part Navigator and on the screen.  And it will remain that way until you reverse the process by selecting the same feature and picking the 'Make Sketch Internal' option.

And if you don't want this behavior where the Sketch is made internal automatically you don't have to go to Customer Defaults to change that as it can also be set in Preferences -> Modeling.

And one other thing, this is NOT a "problem" which persists in NX 8.0 or any other release.  We explicitly changed this behavior several years ago at the specific request of a large number of users, particularly those who were transitioning from I-deas as well as some other Sketch-based modelers where this was already the default behavior.  At first we made it only an option that you had to turn on, but we soon discovered that most people who tried it liked it, so it's now the default behavior, but you can still change it as has already been mentioned.  So, it's NOT a problem, but if you don't like, simply turn it off.  But I would stick with it a while since this cleans up your part navigator and in the end, when you actually NEED to see the Sketch it will be there for you to access it without any extra steps on you part.  After a while, you'll wonder how you put up the old way (I had to go though that transition myself).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Sketches hidden in bodies

(OP)
Thanks for the replies, but I'm speaking about the visibility of sketches that reside inside the volume of a body in shaded mode. Yes, first you make the sketch external to the feature to make it visible in the part navigator, but that doesn't help the problem, the sketch is still invisible in the viewport!

RE: Sketches hidden in bodies

There are two things you can try.

If you're talking about seeing the the complete highlighted sketch when in a fully-shaded view, there's on icon on the selection bar labeled 'Highlight Hidden Edges'.  Toggle this icon ON and then selected curves/edges of objects will be visible even through a shaded model.

Now if you're looking for something where you can see the sketche curves even if they're NOT selected, try toggling ON the 'See-Thru' mode (it's an icon on the 'View' toolbar).  There are 3 styles of 'See-Thru' and for this situation, you best bet will be the 'See-Thru Shell' mode.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Sketches hidden in bodies

(OP)
I toggled on "See-Thru All", then chose the "See-Thru Shell" in the drop down list. Yes, now I can see the sketch inside the body, but the shading quality is not as clear, it looks more like a fuzzy, translucent looking body, not very realistic, which is a shame.

RE: Sketches hidden in bodies

OK, try this...

While this is not quite what you asked for, it just might work for you.  When in the 'See-Thru' mode, activate the 'View Pop-Up' menu (press MB3 over some 'white space' on the screen) and select...

Rendering Style -> Wireframe with Hidden Edges

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Sketches hidden in bodies

(OP)
What that does is simply making the object non-shaded. The sketches, however, appear very clear, but that's not the issue. I don't mind if the sketch in the body appears dimmed, but the shaded body itself should be realistic (not changed in appearance from the shaded view).

Actually, it seems the philosophy of NX is that anything inside a body should be hidden as if it was a real object. So the way to make sketches inside the body visible is to make the body transparent, which can be done by applying transparency to the object or toggling see-thru mode. However, this creates an unrealistic shaded body. What NX should do is add a mode where the body continues to have the exact same appearance as a shaded model, but makes the sketches inside the body "overlayed" on the shaded model.

In the attached image from Solidworks the sketch circle resides completely inside the body, but is still perfectly visible, allowing the user to click it to create an extrude, cut or leave it for future reference.

RE: Sketches hidden in bodies

This is a shot taken from NX, albeit with the sketch selected and the 'Highlight Hidden Edges' option toggled ON:

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Sketches hidden in bodies

(OP)
Nice shot, however as you say, you only see the sketch when you select it in the part navigator. That means you have to click EVERY sketch in the part navigator until the sketch you're looking for is highlighted. Or you can move your mouse around in the graphics view like a blind man until the invisible sketch is highlighted. The sketch needs to permanently stay visible.

RE: Sketches hidden in bodies

Or you can use the 3 or 4 other suggestions I've given you!!!!!

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Sketches hidden in bodies

Can imagine how sloppy a file would like if you had 20 sketches all viewable through a solid????  Doesn't sound like a clean way to work to me.  

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

RE: Sketches hidden in bodies

(OP)
wackolacko, let me ask you something. Why are are sketches that reside outside a body visible, but sketches that happen to reside inside a body are hidden? Is there any reason for this inconsistency? And if you had 20 sketches inside a body, and another 20 outside the body, the outside sketches would still be visible. The part would still look sloppy, but even worse, it would be confusing because you can't see the remaining 20 sketches!

Another thing to keep in mind is that sketches are not features. They do not in themselves influence how a part looks. Therefore, different visibility rules should apply. For example, a cut that resides inside a body is invisible and this is how it should be. But there is no reason that a sketch that resides inside a body should also be invisible, because the sketch itself does not affect the appearance of the part. The sketch is there for future operations, therefore it should be visible at all times!

Now, if the part has too many sketches that clutter the view, simply press ctrl+w and toggle off visibility for sketches.  

RE: Sketches hidden in bodies

Shaded faces hides the stuff behind them, hence our introduction of the 'See-Thru' mode.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: Sketches hidden in bodies

"Why are are sketches that reside outside a body visible" - answer is obvious

"Another thing to keep in mind is that sketches are not features." - really???? last time I've checked they are

I just prefer keeping my files organized, named sketches on separate layers (categorized), feature groups, etc...A little organization goes a long way and I've never had an issue with not being able to see sketches...would that be nice...could be, but then for people who don't want every sketch visible through a shaded body they would have to hide/show all the time.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

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