Supression by Expression - Undersized Holes 1

[TylerCandela]

Hello,

I'm new to the forums, so forgive me if this sort of inquiry is out of place, or out of line..

Part of my daily responsibilities include the preparation of plate files for exportation in .dwg format. These files are sent to be flame cut, and are subject to an array of limitations.

I feel that our current method of excluding undersized holes (>2") can be improved upon. Our current procedure is as follows -->

1.) Create a wavelinked copy of each individual plate.
2.) Create section curves (placed with pocket violation, and chamfers considered)
3.) Create a new sheet, and insert a base view for each plate. (top view)
4.) Perform a view dependent edit, and remove all undersized holes, and pockets. Text and Dimensions are inserted thereafter.
5.) Export .dwg

Unfortunately my superior has limited knowledge in the area of feature suppression(and frankly seems hesitant to even consider using it). To get to the point, I'd like to somehow temporarily suppress all holes measuring less that 2.00" in diameter, insert text and dimensions, and export the required .dwg. After this is completed I'd need to unsuppress the previously suppressed features.

I know that this can plausibly be accomplished through utilization of NX's Journal (or macro?) feature, but I haven't a clue on where or how to start.

Any suggestions would be greatly appreciated.

Thanks!

Tyler Candela


Example of a typical plate file attached below..

 

[TylerCandela]

To clarify,

The insertion of text would be in annotation / note form, and would need to be added while in drafting mode (along with dimensions of the width and height). This would obviously require a switch into and out of drafting mode.

If there is some way that this text could be generated by these dimensions, or properties in the assembly or part navigator that would be AMAZING.

I apologize if any of this is unclear, and I'd like to you to know that I do not expect anyone to complete this for me. I'm not seeking an easy out, just some direction as I have zero experience in this area.

Thanks again,

-Tyler




Tyler Candela
CAD Operator
NX 7.5

 

[JohnRBaker]

Suppress-by-Expression is what I'd do, but if your goal was to supress all holes under a certain size, instead of suppressing the hole features themselves I'd use the Synchronous function 'Delete Face' using the 'Hole' option where I can specify a minium size for the faces to be deleted. Then I would use 'Suppress-by-Expression' on that single 'Delete Face' feature, only in this case 'suppressing' the feature will cause the holes to appear and 'unsuppressing' it will hide the holes.

As for the notation linked to the dimensions of your plate, you can use either Drafting notes or PMI text and reference Expressions used when creating the plate feature.

In the attached example I did all of the above (using a PMI note).

To see how it works look at the features and try setting the suppress expression to '0' for 'unsuppress' and '1' for 'suppress' as well as edit the size of the plate.


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[TylerCandela]

Thanks a lot John!

In time I'd like to figure out how to insert dimensions via macro or journal functions using the outer most points in x/y. Hopefully then I will have also learned how to create a notation driven by these dimensions.

I'm sure you'll see more of me in the coming weeks (I apologize in advance). Any further suggestions would be greatly appreciated.


Tyler Candela
CAD Operator
NX 7.5

 

[vrishraj]

Hi John,

OOTB question, is it possible to remove only the supress by expression option attached to the feature? or need to delete that feature and recreate it to remove supress by expression.

Raj
NX 8.5

 

[JohnRBaker]

Just go back to...

Edit -> Feature -> Suppress by Expression...

...and set the 'Expression Option' to 'Delete for Each' and select the feature(s) that you wish to remove the 'Suppress by Expression' status from and hit OK.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[vrishraj]

Thanks John,

I think, I have missed those expression option selections. Thanks.

Raj
NX 8.5