Hole Feature: Extend through start

[elitetux]

I think I have a pretty unique situation but I was wondering if there was another way about this. I am using NX 9.0.3.4.

I have a conical body that is split down the middle into two bodies. I want to place holes that are radial to the center of the part but are tilted back axially (ie: not normal to surface). If I chose to not use the extend through start I am left with a sliver of material..so I check it on and no problem.

The problem really starts when I try to array a feature group of a few holes holes around the part where the subtract will apply to different bodies..which won't work with the subtract Boolean operation in the hole feature.

Normally I would say no problem - I will just set the Boolean to "None" and then subtract the holes after the array, but setting the Boolean to "None" removes the "Extend Start" option. My only solution at this point is to add an offset point above the surface to the sketch that controls the hole feature.

Is there a better way to do this? I would love to see that "Extend Start" feature with the other Boolean options with the hole feature in future NX releases.

Regards,

- Geoff S.

 

[JohnRBaker]

Can you provide at least a picture of what you'e attempting to do?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
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[Toost]

Maybe not that funny as workaround, but i guess that you can use a Move Face / pull face/ Offset face/ etc on that top face of the "non-subtracted" hole instead of offsetting the point.

Or, Can you create a new "hole to copy" in the second body, and then keep the subtract on both?
- The workaround with the fewest extra steps wins...


Regards,
Tomas

 

[elitetux]

See the attachment for a quick picture of a simplified version of the part. I am trying to array that hole around 180 degrees to the other body. I think the workaround would be to set the Boolean for the hole to none and then extend the face of the hole with "Offset Face" and then subtract from each of the halfs separately. It would be nice to see that "Extend Start" function in a future release for the other Boolean operations..or maybe a way to tell the hole to go a distance in either direction similar to the Extrude operation.

 

[JohnRBaker]

Is this the sort of thing that you're looking for (see attached example)? Note that I used the Datum Plane as my reference 'face' and then used a vector, in this case the Datum Plane, to define the direction.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[elitetux]

Yes similar to that..but we are using gage points on a surface to start the hole and the cylindrical body is made of two linked bodies so it isn't just one solid body. When you start the hole from the gage point on a cylindrical surface you can easily set the hole to "extend start" so it won't leave a sliver of material from the start of the hole. The problem is when you need to apply the hole in a pattern over two bodies.

 

[JohnRBaker]

If you're using linked bodies, why not unite them, create your hole and then the pattern, and follow that by then splitting them apart again at the end?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[mmauldin]

Can the bodies be united then split after adding the hole patterns?

 

[elitetux]

Unfortunately there are about 1200 features before and about 900 features after these holes in the part. They are linked bodies created in the very beginning of the tree. We have a work around by offsetting the start point off the surface and setting the Boolean to none and subtracting from each body afterward. I just wasn't sure if there was a more "official" way to do it or if there were plans for a fix in future nx releases.

 

[JohnRBaker]

If the 'mating faces' between the two bodies are planar, this would not be hard to do.

Note that you say these two bodies are linked. Are they WAVE linked in from another part file or are they Promoted Components? If you're adding this many features to bodies which were originally modeled in other part file but have now been placed together for further machining operations, Promotions might be you best bet.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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