subtracting non touching solids

[filbbb]

when i subtract 30 taps(coned cylinders) from a solid, and one is not touching the solid, it will still remove the solid. in nx3 if the target didnot touch the tool...the tool would stay and not be removed. in nx7.5 it is still pArt of the "subtract" but there is no "flag" to let me know it didn't touch.

 

[Walterke]

good to know.

NX 7.5
Teamcenter 8

 

[jerry1423]

yes, good to know ~ But why are you subtracting a coned cylinder to make a tap?

 

[filbbb]

just an example. we have many costomer that have multaple different standards for tap,screws,dowels...ect....we just insert the screws as we go / at the end of a job.

 

[JohnRBaker]

in nx7.5 it is still pArt of the "subtract" but there is no "flag" to let me know it didn't touch.

Actually there is

After you complete the operation, which BTW is considered as completely valid, if you look at the Part Navigator you will see that the feature will have a little Yellow 'alert' flag on the feature Icon, and if you allow your cursor to hover over the name of the feature a message will appear indicating something like "One of more tools did not intersect the target." Now you can also turn on an 'Alert' column in the Part Navigator and this message will be seen there as well.

BTW, just so that you know what's actually happening here. If you had only ONE Tool body and it missed the Target the Boolean would fail. Also if there were multiple Tools and and they ALL missed the Target it would once again fail. However, if there were multiple Tools and at least ONE of them did intersect with the Target then the Boolean will complete with the only feedback being what I described above in Part Navigator. The rational is that since at least one of the Tool bodies did result in a valid result, we're NOT going to cause the enter operation to fail. Besides, this makes update more reliable since the condition where one of the Tool bodies no longer intersected with the Target, but others did, might be the result of some edit operation so again, as long as at least a Boolean CAN be performed, we're not going consider it a failed update.

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.

 

[filbbb]

Ok I see what you are doing by adding the alerts column & the little yellow "!" by the check box. In nx3 it just wouldn't subtract that particular solid but would subtract everything else that touches. Every time I subtract I have to be careful not to pick something that I know don’t touch (on a different "z" plane or anywhere in space)? My opinion (and I know how opinions work) is if it don’t touch...leave it there or even better yet, show me that it don’t touch and I can de-select it. If I can de-select the solid that don’t touch, it will help even more on the “updating” as there is less solids right? Then all the alerts & yellow”!” would go away?

In nx3 I would subtract my screws (hundreds) by clicking "select all" after filtering my color for taps. If the tap didn’t hit the target then it went to another plate/casting and I continued.

The part navigator cannot be sorted like the Assy. Navigator. If I could sort by alerts it would be easier to find these issues.

Ps. what’s BTW?

 

[ewh]

"BTW" is "By The Way"...

If you are concerned about being able to use the tools for futher operations, why don't you just set it so that they are kept? That way you could still subtract all from whatever solid you are working on, and the tools that would not have been used in any one operation would still be available for another operation.

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

 

[filbbb]

then in order to remove the tool from the file i would have to remove parameter from the target.

 

[Toost]

We are missing a major difference here, which might give the reason for the different behaviour in NX75 vs NX3, If one subtracts 300 bodies in one operation in NX3, you get 300 subtract features ( 299 since 1 failed) In NX75 you get 1 feature that still contains the 300 tools, even if one body misses the target.
This way the model is far more stable when editing, move the 300 toolbodies closer to the target in NX3 and the missing feature is still missing. In 7.5 is will appear as soon as it can.

 

[JohnRBaker]

Toost got it right. The primary reason all of this Boolean behavior was changed, i.e. single feature with multiple tool bodies and allowing tool bodies to not intersect with the target, were all done to improve the robustness of the original model as well as the reliability of subsequent updates.

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.

 

[filbbb]

makes sense

thanks again