Unite/Subtract Issue!

[eddyder]

I'm trying to subtract a solid body from another solid body (which do intersect but I still get this error message "Through face does not intersect path of the tool")

 

[NutAce]

I see this small circular face on the top. try and offset that on the tool such that it will stick out..

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5

HP Zbook15
Intel(R) Core(TM) i7-4800MQ
CPU @ 2.70 GHz Win7 64b
Nvidia K1100M 2048 MB DDR5

 

[Xwheelguy]

To expand on Ronald's suggestion, it's "preferred" modeling practice to extend all solid tool bodies beyond the target bodies in order to avoid what's called Non-Manifold conditions, which is what is showing in the area Ronald is talking about. Same goes for sheet bodies - don't model them meeting at a shared edge, extend them through each other and trim them back.

You're going to wonder why and the simple reason is due to the modeling tolerances being used, non-manifold conditions can make the system come back with the error message you're seeing. Just make sure you always overlap, extend beyond what is necessary (by a few mm or an inch) and you'll be fine in the majority of cases.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[Miyamoto12]

I alwayw thicken into the other body, then subtract to be sure

NX 10

 

[cowski]

All the above is good advice. If it doesn't help in your case, run the 'examine geometry' command. Sometimes a geometry error (consistency error, self-intersection, etc) will cause later operations, such as a unite or subtract, to fail. If a geometry error is found, it will need to be corrected.

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