Subtract Outside of a Circle

[BOPdesigner]

I sketch a circle on a planer face and then want to extrude it into the part with the subtract boolean. Obviously this creates a hole in my part. My desire however is to subtract material outside the circle leaving a solid on the inside, like a boss. Is there a slick way do to this without sketching a 2nd circle or another joined profile that encompasses the original circle and all other features in that plane of the part?

 

[SiW979]

Have tou tried the intersect which is also on the boolean drop downs along with unite, subtract and create? This will leave you with only the material where the two bodies intersect?

If you could post an image or model, then that may help me understand a bit more.

Best regards

Simon (NX4.0.4.2 MP9 - TCEng 9.1.3.6.c)

http://www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

 

[mmauldin]

Sounds like you need to do an extrude with a single sided offset. This will create a "ring" of material that can be subtracted.

 

[jerry1423]

I believe there is an easy way to do what you have described in SolidEdge, but not in NX.
The above two postings have good solutions

 

[BOPdesigner]

The extrude with intersect cuts out everything past the cut extrude stop length also. Here is an example part image:

http://science.gcc.edu/mece/projects/2003/Mini-baja/Image7.gif

But instead of the hole in the center, I want a post sticking up and then use the extrucde trim the features back around the post to the front surface shown there.

 

[GBOLD]

You can draw a set of curves outside the area you want to cut away, if I understand what you are after.

 

[JohnRBaker]

Can you provide, even if it's a hand drawn sketch, of what you're looking for?

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[Jaydenn]

I have a feeling this is what BOPdesigner is speaking of...
(see attached)

Forgive me if I am wrong!

J

 

[BOPdesigner]

Simple case attached in NX 6 format. Basically I was just curious if there was a way to achieve that result without having the outer circle on sketch(4). Cutout (boolean subtract) everything outside the single smaller circle. There could be ribs or other features on the base cylinder that I want trimmed down also.

 

[JohnRBaker]

As was already suggested, you could use the 'Two-Sided' Offset option with the Start set to 0.0 and the End to a value large enough to cover the area needed, as shown in the edited version of your example which is attached below.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[mmauldin]

Yes, two sided was what I meant to say. Don't know why I said single sided, must be an age thing.

 

[BOPdesigner]

That method works thanks. I was thinking that there might be a way to flip from the inside to the outside of the circle for the extrude with subtract.

 

[hudson888]

Just going by Jaydenn's image I would add that you could achieve that same kind of result by creating a shorter base block extruding the shape without offsets and uniting the two bodies together. That would be more conventional and robust. The reason to mention it is that in the case of a circle you will never have difficulty creating the offset, but for some profiles you're eventually likely to strike a concave corner that is too tight to allow an offset large enough to subtract from the existing block. Since either case requires the same number of features and effort I'd probably defer to the first method where possible.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum