It's one of those things that I don't understand why it got programmed like it did. Meaning why didn't they just include a "hide tool" selection box for thicken and split body commands?
Actually there is, but it is a very generally purpose behavior which is why it's OFF by default, but I'll let you try it for yourself and you can decide if you wish to leave it ON, or manage the display of 'used' objects yourself. Note that when we first added this option in NX 2, I was an instant and enthusiastic supporter, telling anyone who would listen about it. However, over time I've mended my ways and have turned it OFF on my system and now only talk about it when explicitly asked for something along these lines, like right now ;-)
OK, there is an 'option' which is located in a rather obscure place, which at first I questioned myself but I was warned by the development supervisor responsible for this area of the product that I should try it first before I got too concerned about how hard it was going to be to find, and I see now that he was speaking from a position of knowledge, but I digress...
First you need to understand the concept of an 'Unused Item'.
Basically when you're creating some SOLID model there are all the things which make-up the solid and then there's everything else. Now when you look at the Part Navigator and it's set to 'Timestamp Order' ALL Features are seen in the order in which they were created and non Features (like dumb curves and non-associative points) are not shown at all. In this mode the concept of an 'Unused Item' doesn't really have any meaning, however if you were to toggle OFF the 'Timestamp Order' and enter what is known as 'Model Mode' you would see individual SOLID bodies as part of something called 'Model' (BTW, this name refers to the 'Model' Reference Set which by default, all of the Solid Bodies are automatically added to. You could also say that 'Unused Item' referred to something as NOT being part of the 'Model' Reference Set) as well as a couple of other new items, one where you see a listing of any non-Model Reference Sets and something called the 'Unused Item' folder, where any geometric object (even dumb ones) not included in the 'Model' Reference Set can be found. Now as you create any non-Solid geometric object, whether it's a feature or not, they are both visible and added to the 'Unused Item' folder.
Anyway, there is an option which can be set which will automatically 'Hide' any 'Unused Item' which is referenced (i.e. 'used') by some Feature during it's creation, EVEN if the resulting feature/object is NOT a Solid body. Of course, if the resulting object is NOT a Solid it will also end-up in the 'Unused Item' folder, thus making it a candidate for automatically being hidden IF it's ever referenced during the creation of some other feature.
Now examples of this are sheet bodies or datum Planes used as a tool when trimming a solid, or the child sheet body which I created a Thicken feature (well there goes your problem), but it doesn't stop there. It also includes the two curves which I create a Bridge Curve feature between, or all of the Points I select when I create a Spline. It also includes the previously created Sketch I use to create either a Solid or a Sheet Body with, only in the case of the Solid result, it gets added the Model Reference Set while the Sheet Body becomes a top-level item in the 'Unused Item' folder.
Now this will give you the behavior that you're looking for, but the PRICE that you pay is that EVERY object NOT part of the Model Reference Set, which you select as reference for some feature creation, will automatically be hidden from view. Now you may at first say that you're willing to pay that price, but after awhile I (and many others as well) have found this to just too much of a hassle and come to the conclusion that we will 'manually' manage the 'tool' objects on our own as we go along (now remember, this has no effect what gets or does not get added the Model Reference Set as that's controlled by another set of options).
So where is this obscure place I can find this option at?
Open your Part Navigator and place your cursor over some 'white space' and press MB3 and from the pop-up list select 'Properties'. There you will find an option titled 'Hide Objects When Used'. Toggle it ON and you will have the behavior which I described above. Also note that this can be turned ON by default at...
File -> Utilities -> Customer Defaults -> Gateway -> Part Navigator
Well there it is, perhaps one of the least known options in NX which can be turned on from a dialog. Give it a shot and let me know if this is what you were looking for.
And one last bit of information, if an item, such as a Sheet Body used as tool in a Trim Body feature, happened to be part of the Model Reference Set, the setting of this option will have NO effect whatsoever on the display of the item being referenced, i.e. it would remain visible.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
To an Engineer, the glass is twice as big as it needs to be.
![[wink]](/data/assets/smilies/wink.gif "[wink] [wink]")
I too understand quiting an addiction! Not smoking but Getting that Dang Monkey off my back made me grumpy too! Keeping it off is even worse! Thanks for the help!