Suppression by expression in part family

[ashivu123]

I have bolt family members in which some of them having Holes in the head and some of them in shank and some bolts are undrilled. I have controlled the with suppression status to turn ON and OFF (0, 1) with respect to their numbers.

Initially I have not selected BOLT_HEAD_ DRILLED AND BOLT_SHANK_DRILLED suppression status to chosen columns and entered only Diameter to create parts. Parts were created but failed to update the Hole feature in the child part.

Later I have included suppression status to chosen columns and created parts, parts are created with no errors and hole feature updated in child parts.

Is there any suggestion how can avoid entering the suppression status in excel sheet. I want limit the suppression status in the model itself.

 

[JohnRBaker]

To what end? I ask this because once a family member has been created it is 'Read Only' and can never be modified and then resaved. And before you think that you can just go into Windows and change the read/write status of the part file, that won't work since family members are 'Read Only' at the NX level meaning that there is NO way for anyone to make any permanent changes to a family table part, period.

Now if your issue is that these holes are actually being drilled after the bolt has been assembled into your product, that can be done using the 'Assembly Cut' functions which will allow you to create tool bodies in the context of an assembly and then Boolean subtract them from the Components of an Assembly to represent holes 'drilled' at Assembly in the real world. And you don't need 'Read' access to the Component parts since these tool bodies and the Boolean subtracts (AKA the 'Assembly Cut' features) only exist AT the Assembly level.

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.

 

[phillpd]

You can simply make use of an "if-then" expression that will suppress the feature based on another expression value.

Let's assume we have the suppression expression "HeadHoleSuppression" and the Hole Diameter expression "HeadHoleDia"

HeadHoleDia=3
HeadHoleSuppression=1

HeadHoleSuppression=if(HeadHoleDia==0)0 else 1

Now, the actual expression controlling the Hole Diameter would need its own expression to avoid being set to 0. For example ... p6=if(HeadHoleDia==0)2 else HeadHoleDia.

In the above, the value of 2 is just a default value to ensure the diameter is valid.

NX 6.0.5.3
NX 9.0.1.3
Windows 7 64

 

[ashivu123]

Hi Phillpd, Thanks for replay

i am getting error while doing expression getting Syntex error.
Head hole diamter is having tow values diameter .046 and .070 (For AN3 to AN4=.046 and for AN5 to AN20=.070)
Let me know how can i writr if condition for above.

Thanks.

 

[ashivu123]

Hi John,

Holes are not drilled in the assembly level. They drilled in the part level itself. The reason i asked is in the spread sheet I have 4 columns for controlling these holes on Head and shank. I like to know whether these can be limited only 2 columns such that only entering hole dia in the row. How it can be controlled by giving if condition?

 

[JohnRBaker]

Are you aware that you can control the suppression of more than ONE feature using the same expression? When you use the Surppress by Expression function and if you select more than one feature you will be given the option of creating individual expressions for each feature OR using the same expression to control all the features selected.

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.