Extrude with single-sided offset collapsing face

[DHuskic]

Hello,
I am attempting to create an extrude with single-sided offset but it is collapsing the face sometimes and only building one of the collapsed regions. Is there any way to force it to build all of the regions or switch which region it builds every time? See attached image for sample

NX 9.0.3.4 MP13

DHuskic
Nx9.0

 

[Xwheelguy]

I'm thinking that ball-end slot nearest the middle of this "pad" area is too close to the outer perimeter for the offset to work in all 3 areas that you're expecting to appear in the preview. Try selecting the curves such that it's not everything at once. The 2 areas that appear to be mirrored might be able to be done all at once, but that left-most area will have to be done separately.

See the attached image for what I'd try - might have to be 2 Extrudes (the right-most areas with blue outline & then left-most in red.

Extrude_wOffset.PNG

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

 

[cowski]

I'd suggest doing the offset in a separate operation(s). Extrude the face up the desired distance, create a datum plane along the axis of the slot, split the body of the extrude into three parts, and apply the offset on each of the resulting bodies.

www.nxjournaling.com

 

[DHuskic]

I am using the Face selection intent to select all the edges of the face highlighted below:

If I do a regular extrude normal to the face, and without any offset, here is the result.2. No offset example.png

When I start putting in a negative single sided offset, the offset causes the edges around the ball end slot to collapse on the edges going on the outer perimeter of the face. This collapses the offset and instead having multiple extrude bodies as results, it only chooses one region.

When I increase the offset, the region changes for some reason.

This is the result that I would like, for all 3 regions to be extruded:

DHuskic
Nx9.0

 

[cowski]

Split the extrude into three bodies before applying any offsets.

www.nxjournaling.com

 

[JohnRBaker]

I suspect that you will find that while you can Extrude a profile that will result in a feature which contains more than one 'body', this only works if the multiple bodies are NOT the result of an 'Offset' operation. Look at the what the results would be if you HAD created the model using three separate Extrudes, each with an Offset. The result is three separate bodies. And don't expect GTAC to agree with you that this should have worked. This is a pathological situation that's beyond what the software was ever intended to do.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
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[Xwheelguy]

After looking into a part with similar features, I'm going to side with cowski's advice of Extruding without Offset (and without Unite), Split the Extruded body along the shallow ball-end slot, perform an Offset Face, and finally Unite at the end.

A few more steps, but nothing that is overly cumbersome, in my opinion.

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