nx7.5 Deleting target feature? 1

[SDETERS]

I am in the process of modeling a die cast housing using solid bodies. In I-Deas we usually modeled the outside of the part then the inside of the part then cut the inside from the outside. In Nx I am doing the same thing but using solid bodies instead. Which it is working nice until now. For the Solid body I am working with I have done probably 10 subtracts and or unites to a single target of a sweept feature. I have done the unites and subtracts in the extrude, revolve feature form. In the part navigator the unites and subtracts are not individual steps. Now when I go delete this sweep it deletes all of my other features that was tied to that one sweep. OUCH.
What is the best practice for modeling with solid bodies. Is it better to model all of the features, and then do many unites at the end? Is there a switch that will allow me to delete the target with out deleting all of its children and let me go back in and choose a different target? This will also help with some CMM issues we are having but that is another issue all together.

 

[JohnRBaker]

It sounds like want to now delete the Swept feature without deleting any of the tool bodies which have been used to modify (add features) to the original swept body (not sure why you want to delete it without deleting the other features, but I'll assume that you know what you're doing ;-)

OK, there is something which you can do, even after you've gotten to where you are. All of those feature operations, where Booleans were performed but which you can't see in the Part Navigator, you can go back and edit the added feature changing the Boolean option to 'None' and then performing the Boolean as a separate operation which will now appear in the Part Navigator. Now if you do this for all of the features 'attached' to the swept body and later you wish to delete that original swept body but NOT the 'attached' features, all you have to do is go into the Part Navigator and DELETE the Boolean operations (but not the extrude/revolve features) and you will now the 'attached' features as standalone solid bodies but no swept solid body.

An alternative approach, if there was a real expectation that when you got done that you actually would be deleting the original swept body while wishing to keep all of the 'attached' extrude/revolve features, would be that while you were performing the explicit Boolean operations, that you go in the 'Settings' section of the Boolean dialogs and toggle ON the 'Keep Tool' option. What happens now if that the Boolean operation will be perfromed but that tool body(s) will NOT be deleted but rather will be copied and then the Boolean performed. Now just hide the tool bodies and later if you need them again, they will still be there and if at the very end of your job you decide that you will never need them, just unhide all of them and delete them.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

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[SDETERS]

Good Information thanks. Also we found a setting that when you delete the feature it will not delete the child. Go to file utilities and customer defaults. Then General then Delete and suppress tab, and click off delete child features. This deletes the feature but gives a warning of all the child features that will be affected. Which this will also help with the CMM issue we are having with the parts we are brining over from I-Deas.

(not sure why you want to delete it without deleting the other features, but I'll assume that you know what you're doing ;-)

We wanted to reuse this part for a different part in an assmebly. we did not want to remodel everything, and also did not want this sweep in this part. Which in this case was the very first feature in this part.