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Trim Body Command using Surfaces in NX 10.0

Pioneer
Pioneer

The translucent region (say V1) is a solid cuboid body, extruded from the bottom face of the “F”

The opaque solid cuboid (Say V2) is the extrusion of a different bottom face (the one of the smaller horizontal beam making the F)

V2 is already subtracted from V1 to avoid redundancy.Trim1.png

 

 

I want to trim V1 so that the area outlined in black, gets removed (pic below).

 Trim1.5.png

 

To start, I extracted the faces (as in pic below) and sewed them:

 Trim3.png

I then used “Trim Body” Command, selected the V1 and the sewed faces as trimming faces and I got the desired result:

Trim4.png

I got this same result even if the sort of bumped up face in one of the sewed faces was just a plane face.

My query is I fail to understand is how the Trim Body command is designed to work? Like the normal to one face is in a different direction and another face is free form with many normals, then how does the trim body command understand what volume to keep and what to remove for this case and in general?

I wish to understand this so that I can generalize this concept to trim bodies, using API,  for the application I intend to develop.

7 REPLIES

Re: Trim Body Command using Surfaces in NX 10.0

Phenom
Phenom

In your description there are many aspects to see:
First: the command extract face includes the chain face option in that way you do not have to use the sew command.
Second: the trim command has had a great evolution in the latest versions so the results may not be those desired.
For example up to NX7 version, if I remember correctly, you could not cut-trim a solid if the result gave more solid (see image).
Other aspects are long to explain, for example, the possibility of replacing the trim command with the replace face command, and so on (see other image).

 

Ciao

Re: Trim Body Command using Surfaces in NX 10.0

Phenom
Phenom

To better explain my second point in the previous post I attach the image:

Ciao

Re: Trim Body Command using Surfaces in NX 10.0

Phenom
Phenom

It works because you've subtracted V2 from V1 prior to the Trim Body.  I'm a fan of simplifying things as much as possible, so I see no need to use Extract Face at all - just use the "F" body's 2 faces as the tools - that's a valid method, although as you already see, not the ONLY method that will work.

 

What I don't understand is why you say you want the lower V-shaped area removed from V1 (see your 2nd image from the top) yet you work on the upper side of the lower vertical beam as you call it.  If the area you want removed is correct in the second image, just use the lower angled face (left-most vertical "beam") from the "F" after the subtraction (V2 from V1).

 

My movie will show V1 results with 1 Trim Body as you describe (without the bulging surface) and then a second result as you describe in your 2nd image.

 

 

-Tim

Re: Trim Body Command using Surfaces in NX 10.0

Pioneer
Pioneer

Thanks for detailed response and the video Tim! You are right, I could have just used the second approach and selected the slant face below the lower beam of the "F". But, if you look closely, that keeps a portion of the extrusion inside the "F" body. I mean to say, if you check the volume of the extrusion after all trimming operation, in method 1 and compare it with method 2, the volume of extrusion will be larger in method 2 since a portion is inside the main "F" body. 

This might lead to some errors when processing such CAD files. 

Re: Trim Body Command using Surfaces in NX 10.0

Phenom
Phenom

Yes, that leaves a portion inside the F body - because that's what your 2nd image shows!  "I want to trim V1 so that the area outlined in black, gets removed (pic below)."  Then in the very next image you show something completely different - I believe things are a bit out of order compared to what you're wanting or expecting but no big deal.

 

Attached is another movie in which I am assuming you want what's shown done - again from what you've posted, it's my best guess because of that 2nd image not being very clear to me at least.  No need to Extract the faces unless you're adamant about using a surface as the tool trimming object - faces from solids serve the exact same purpose.

 

Just think of Trim Body as a way to use tool sheets OR faces to chop away from a solid (or another group of sheets in some cases).  The red arrow is the key, as that is what determines which sides are kept - don't worry so much about how surfaces might bulge and the vectors on every little point - that's the power behind Trim Body - thos are taken into consideration within the command itself - it will match the tools (within the modeling tolerance if needed).

 

Hope this helps.

 

 

 

 

-Tim

Re: Trim Body Command using Surfaces in NX 10.0

Pioneer
Pioneer

Thanks Tim! Yes, that's my bad of not showing the image properly. But I get your point. I did try selecting faces of the solid body to do the trim, but somehow that didn't work. I will check back if there was something I was missing. 

Re: Trim Body Command using Surfaces in NX 10.0

Phenom
Phenom

Without your original part, it's just a guess as to what might have been different.

 

When using Trim Body, the red arrow indicates the side to be REMOVED from the target body.  You just need to make sure that your tool bodies or faces are at least touching, if not extending through or past the target body.

 

In my example, everything worked because the geometry was quite simple and except for the bulged area, all planar - more complicated shapes/surfaces/faces might give you issues with Trim Body - it just all depends on how it's all coming together prior to the Trim Body.

-Tim