Sheet flanges uniting

[Rich944]

Morning all,

I'm creating a sheet metal part and have a problem. The part is made up of 90° flanges that fold on top of each other (not intersecting tho).

As the flanges touch each other they become united, ( both edge faces of the flanges highlight at the same time), I think this is causing me problems when I want to unbend the flanges and also put a hole through both flanges (they are riveted together).

Is there any way around this, other than leaving a small gap between the two flange faces?

Or maybe there is another way to model this?

Thanks in advance.

Katt

 

[hudson888]

Katt,

I would go with the very small gap. It may not be the purist solution but I can't see the point in fighting it for what it is worth.

Best Regards

Hudson

 

[Rich944]

Thanks Hudson,

I thought that might be the case, just didnt want to tarnish my model with odd dimensions

 

[JohnRBaker]

Yes, but in reality, if you manufactured that part there would probably be a very small gap there as well.

Now you're not talking about a 'Hem Flange' are you, where you fold the flange over onto of itself to make a smooth, stiff edge? If so, we added support for that in NX 5 and while the opposite faces do actually touch each other, it remains as if it had not been merged into a single solid.


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/

 

[Rich944]

Hi John,

No not a hem flange, the two flanges come from the side edges of a 90deg bend, and end up touching faces.

I want to put a hole through these flanges in each corner, some work fine, but the last one keeps giving me "the tool and target do not form a complete intersection" ?? I'm on NX5 btw.

Thanks

 

[Rich944]

This may make things clearer -

http://files.engineering.com/getfil...4-aa52-4124-9474-838470176e01&file=flange.jpg

I want a hole in the center through the two flanges.

 

[Rich944]

http://files.engineering.com/getfil...-6243-4f21-9c47-92fff2ac564d&file=flange2.jpg

This shows another two flanges merged together (which is not what I want), the hole worked that time, but I dont think I can unbend it or produce a flat pattern.

Any advice appreciated!

Thanks
Katt

 

[hudson888]

Katt,

Just to let you know I saw your pictures. I think you've just about formed an understanding of what the system can and can't do in this regard.

Interestingly I created a pair of flange features that apparently touch as sheet metal flanges, the most basic type. They seem to be a special case in that they have zero gap, but don't unite, and they are ideal dimensions. Then I came across you conundrum trying to get a hole through the corner. Try making the first flange, and adding a hole to it, then creating the second flange, and making in it the same sized hole aligned to the first one using point to point method (pre-NX5). I think you'll find that solves your problem.

best regards

Hudson

 

[Rich944]

Thanks Hudson,

I tried your method of creating a hole on each flange, unfortunatly when creating the second hole I got the same error.

How did you have the two flanges touching but not unite? Did you create them with the old style sheet flange within the model app? eg. modeling > insert sheet metal feature > flange. I've just tried this and it works, although when I try the hole - guess what - same error.

Anyway looks like im gona have to redo the whole part! I just suppressed a chamfer and now i get an 'internal error' if I try to change or delete any feature! A few of us here having the same problem, I'm told the only work around is to start from scratch using 'old style' sheet metal features through the modeling app :/

 

[hudson888]

Katt,

Yes the old style flange. I didn't have the full sheet metal license running to test for this, so I just used what was loaded.

Out of interest when you create the second flange is it united to the first, as shown in your image? I can help with some testing up to NX-4 on the full set of licenses if it would be of any use.

Those internal errors are a pest, NX blaming Microsoft for it's problems no doubt.

Firstly you want to try and see if the part clean up will help tick the top four options at a minimum. Try and wind the model back to the start and step forward using make current feature until it goes away if that doesn't work. I keep telling people that I have never yet ultimately lost a model because of this.

Best Regards

Hudson

 

[Rich944]

Hey Hudson,

Thanks for all the advice, I've remodelled the part and my flanges are no longer united now - cos I put tiny gaps in and used old school sheet metal on my part. No more internal errors as yet and the hole went straight through. Just found out that my graphics card isnt a preferred UG one, maybe could have been a cause for these errors.

Katt

 

[hudson888]

Katt,

For what it is worth I have both preferred and non-preferred graphics cards at my disposal and I often advise people to only go for the expensive ones when they have need of high end performance, (ie rendering large complex geometry).

Anyway you graphics card won't affect geometry outcomes in any way. The old school flange is a special case that appears capable of touching without uniting. I haven't tested what the NX-5 sheet metal package actually does, but I think we've learned enough from your experience.

Now the reason I also mentioned about putting in two holes rather than one is that I am guessing it may work more easily for flat patterning. That is if you unfold the model. To be honest I prefer to use the curve flat pattern also available with the sheet metal package which doesn't seem to care how you model the part as much.

Best Regards

Hudson