Hole feature in assembly level / NX1973 1

[IREYES]

Hello everyone,
I have found myself in such a problem using hole feature, commonly in other CAD platforms as Solid Edge and Solid Works you can include holes that you don't want to depict in part level but in assembly level, eg. when you have a weldment assembly that need to be re-drilled after fabrication.
I tried using normal hole feature, and then select the face where i need to locate the instance but seems to have no result,
I'm not sure if i'm using it the wrong way because this is the first time i'm using assembly cut and hole feature at the same time to represent my instances.

What is the process you often use in order to depict this?
Below is attached the warning that i have every time that chose to run it that way.

 

[TheTick]

There are two ways to accomplish:

Use WAVE Link to bring part body into assembly

Use Promote to bring component body to assembly level. (This still works but I believe is obsolete and hidden). Functionally, promote is closer to what you are trying to accomplish.

 

[cowski]

In the hole command, choose the "hole series" type. This will let you create a hole through one or multiple bodies in an assembly. It uses a promote body behind the scenes, so the hole only shows up at the assembly level.

https://docs.sw.siemens.com/en-US/p...5732916.modeling/html/hole_adv_hole_series_ov

www.nxjournaling.com

 

[IREYES]

Sounds good both of your recommendations,
I already tried the "hole series" command but seems that is not going to fit me because I only need to make threaded holes in some tubes, and not a sandwich of parts.
By the way, it tried using promote with no success, my customer defaults is not allowing me to modify the config.
I'm working with the Daimler supplier package for NX and make modification to my customer defaults is not able.

Thank you

 

[Toost]

If you cant create wave links or promotions ,
Then the remaining option is an assembly cut feature, the sad part is that it requires a target body and a tool, where the tool is the "hole".
so the backward option is to first create a hole feature without the subtract option ( will create a "positive hole solid") and then create an assembly cut which subtracts that hole from a linked body.

But, check if you can create a Wave linked body first.

Regards,
Tomas


Never try to teach a pig to sing. I wastes your time and it annoys the pig.

 

[Befuddled]

Hi,

One of my favourite ways is to use assembly Cut. So you don't technically use the hole command, as you will need to model the material you want removed.

Cheers,

B