Hole Series feature failing during update NX 7.5...

[3dr]

I just started using this on a new job. Looked like an attractive tool but the feature is failing after a simple mod to a plate thickness.

Ex:
1. Have a 6 componet ass'y.
2. Used "hole series" to fasten 2 of them together. (From the top level assy)
3. 1/2 fastener...
a. Start tab (clearance hole)
b. Middle tab (nothing)
c. End (tapped hole)
4. Changed the plate thickness with the clearance hole from 1" to 1.25"

The hole series failed and won't update. Its abvious that the plane the points are sketched on didn't move with the face they were attached too.

Any ideas? Can this actually be a limitation????

TIA

Dave

 

[3dr]

Ok, it's obvious after playing around that the face of "start" componet is extracted and thats what the sketch is attached too. That extracted face isn't updating and moving with the face in the componet.

Looks like a failed wave link thats consumed by the hole feature.

Perhaps I'm not doing this right?

Shoule the "start hole" be "in" the componet with the "start" face?

 

[JohnRBaker]

You may need to get your parts to GTAC and have them look at what's happening.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[3dr]

Yeah, maybe so. I worked around it by placing the feature in the part with the "start" face.

That worked fine but it seems to me it should work either way when updating.

These parts were converted from Metric to Inch units right before I started. Maybe there's a modeling tolerance or something like it tripping it up.

 

[phillpd]

3dr,

I can't comment on NX7.5, but with NX6 you have to toggle on the "Create Interpart Link" icon on the Selection Toolbar.

You then click this icon when you create the Hole Series. This will create an associative linked face.

 

[uwam2ie]

there are two way to do hole series,
1.creating in the assembly node
2.creating in one (top) member parts of the hole series
the experience and maybe we discuss the pros and cons of 1,2
advantage 1st the holefeature self acting recognizes the hole member parts.(eye catcher).Disadvantage of this method is editing the feature from one of the holemembers prt no jump to the feature owning part is available as it does in the 2nd way. Another problem could be when you have got a workflow in your company into SW or V5 through step. You can not open the step because of the linked face in the assembly node, you must control your step export settings without faces.

 

[3dr]

I've got a couple of big projects coming up with a lot of fastening. I suppose I'll be an axpert on what all the pros and cons soon enough.

The "Create Interpart Link" icon is always greyed out and I havn't seen any circumstances when I have a chance to toggle it on.

I'll keep an eye out for it and report back later on whatever I consider to be "best practice"

Thanks Guys

 

[phillpd]

3dr,

(at least with NX6) When you open the Hole dialog, that icon will be available for use.