How do I remove trimmed sheet(s) (tool body) from the model in nx6

[ingallspw]

My problem has to do with the "Trimmed Sheet" and "Thicken" commands in NX 6.0.1.5.

In short:
If you look at the attached screen shot, I just want to remove the surfaces completly from the model (not hide) and just keep the solid.

Detailed:
I am trying to "twist and deform sheet metal" and keep the true shape of the twist. I am doing this by creating a surface (larger than needed), trimming it to the true shape, and then thickening it. I hid the surfaces (light blue) but the problem is these surfaces keep popping up their ugly little heads in assemblies, drawings, exports, etc.

Screen Shot:

http://files.engineering.com/getfil...0c-a474-3edbceccab6f&file=remove_surfaces.jpg

Any help would be greatly appreciated!

Thanks,

Keegan
Horton Inc.

 

[ewh]

Try removing the parameters from your thickened body, then delete the sheet.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[hudson888]

You have either to do as described above remove the parameters that derive from those bodies so that they can be deleted. A regressive solution if ever I knew of one.

OR

You could just attempt to maintain your reference sets properly so that in the context of the Assembly reference you're looking at a reference set that only contains the solid. This is by all accounts the better solution. Start by manually removing those objects from the model reference set. and let us know should you continue to have difficulties.

In addition many users place all the construction geometry that they don't include in the finished model definition on to different layers. If the component is loaded to your assembly using the "original layers" method by default then as long as the construction layers aren't displayed then even the odd errant reference set will not trouble you by dispaying extraneous geometry.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[ingallspw]

The problem with loosing the paramenters is I am working on a part that the angle can be changed so I want to keep it fluid.

I like the layers idea as long as it doesn't try to export the surfaces. I'll give it a go and let you guys know what the outcome is.

Thanks!!

 

[cowski]

How you do the translation will determine what gets translated. If I use the stand alone translator it will translate everything in the part file, but if I use the export command from within NX I can pick specifically which body(ies) to export.

There are probably options within the stand alone export program to get what I want but I don't mess with it often enough to dig into it.

Reference sets in the assembly is the way to go to keep the sheet bodies from showing up where they should not. Refer to hudson's post above and the help files.

 

[demco]

The answer is Properly Maintained Reference Sets. Remember, if you are modeling in context of an assembly, and have the Ref Set set to MODEL, everything you create gets added to MODEL. If you however are modeling in the part file (part is Displayed, or in an assembly where teh ALL ref set is active, the MODEL reference set will only contain solids - no surfaces. In that case, if you have solid reference geometry, you would still need to manually edit it out of MODEL.

-Derek

Check out

http://www.spacex.com

 

[ewh]

The problem with loosing the paramenters is I am working on a part that the angle can be changed so I want to keep it fluid.

Knowing that you didn't really want to "just keep the solid", I would have suggested as the others - learn how to properly use reference sets and/or layers.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[ingallspw]

It's one of those things that I don't undersand 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? It's in plenty of other things. Especially thicken...

 

[ingallspw]

EWH, don't take it as me saying it was a bad idea. Actually I'm just thankful for all the help! I probablly would have done that if I didn't plan to adjust it later.

Thanks!

 

[ewh]

No problem. I usually wouldn't have responded like that, but I quit smoking last week and am a little edgy yet.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[JohnRBaker]

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

http://www.siemens.com/plm

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

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

 

[ingallspw]

Sweet! Thanks John! That little tidbit of info is extremley helpful! I shall pass it on to others who may find it helpful here!

Keegan
Horton Inc.

 

[ingallspw]

EWH - 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!