flat pattern visible in assembly

[uwam2ie]

I'm not really familar with Nx6 sheet metall.
We have sheet metall part with some flanges with FLAT PATTERN FEATURE. The curves are transfered into a view and a spe. layer. Working with entire part referenceSet in the assy of the sheet metall part the flat curves were shown. Reference set model fixes the problem. Are there any other opportunities to control the visability of those curves in the assembly or if you add this sheetmetall part master model to a drawing with entire part?
thx in ad

 

[JohnRBaker]

That is what Reference Sets are for, separating that which you wish to see from that which you do not, when you place the Part in an Assembly, whether that is an Assembly of the final product, or whether it's a single level Assembly as used when creating a Master Model Drawing.

Now in the case of a Drawing of the actual sheet metal part itself, with the Solid in the Model Reference Set, create your Master Model Drawing and place the views of the as formed sheet metal model and then to include the Flat Pattern, place another 'Base View' only change the designated named view to the one which was created when the Flat Pattern was defined and place that on the Drawing, so that now you have both the as-formed and the flattened version of the model on your drawing.

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.

 

[uwam2ie]

The drafting problem is that we have a design guideline to use the entire reference set on single part drawings- with the layer visable in view workflow - when needed- view from part we have avoided - I have forgotten the reason why....
thx ( esp. John Baker)

 

[JohnRBaker]

I suggest that you CHANGE your 'design guidelines' so as to take PROPER advantage of the way NX was DESIGNED to be used in the first place.

Also, from what you've stated, it seems to suggest that you be ONLY allowing the use of Reference Sets inside of an Assembly. Is this true? If so, that is the exact OPPOSITE of what Reference Sets were designed to be used for. We do NOT recommend that you ever create Reference Sets in an Assembly. They act as explicit filters and could eventually cause you all sorts of problems which may prove be very difficult to sort out months from now when they start to manifest themselves when and if these Assemblies are modified and updated, particularly if they contain sub-assemblies or these assemblies are themselves used as sub-assemblies.

'Visible in View', while still supported, is considered an arcane function and should only be used IF there are NO other solutions which meet your needs.

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.

 

[uwam2ie]

- we will change our guideline I think,
Reference Set are used - in assembly part we use only entire part no reference Set in assembly level. On the components model referenc Set - on drawing we use the component visible in view as first choise layer visible in view and only as last the view dependent options.
layer visible in view ( only in drawing views)is still heavy in use...

 

[BOPdesigner]

John, you are hinting that 'Visible in View' is on the table to be obsoleted at some point. What are are you intending to replace it with?

 

[hudson888]

I don't think that it can be dispensed with for legacy support reasons. There have always been people who either prefer to use the system in ways that aren't in line with the designer's most earnest intentions. Indeed from time to time it is still as convenient a way to do certain things as any alternative method I currently know of. In that sense what might be called legacy refers to what we still do even now, so I wouldn't want my NX-7 parts to fail in NX-8 any more than I'd want my oldest parts to fall over. For that reason alone I'm doubting that things like visible in view for drafting nor layers can be easily gotten rid of.

Now if they switched off the ability to make new instances of view dependant geometry, or to set up visible in view from within the modelling application then I should not be in a least bit disappointed.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

NO, 'visible in view' is NOT being considered for removal. We have learned to live with it and will continue to do so in the future.

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.

 

[moog2]

when i create the flat pattern in the part, a flat pattern ref set is produced. In the drwg, when i create the views of the folded part, by default the ref set is model, if i then create a new view to get the flat pattern, even if i select a view created in the part, of just the flat pattern, it still only shows the folded part, because the ref set is set on model.
Both folded and flat pattern are to be on the same sheet, the only way i can see i'll get it to work is creare a new ref set with both folded and flat in it (on different layers) and use visible in view, i'm trying to avoid this method from recent thread explanations, but can't see another way?

 

[JohnRBaker]

I have no problem whatsoever doing this.

With NX 6.0.5.3, when I create the Master Model Drawing and I add the Component for the 'a- modeled' views, the system automatically used the 'Model' Reference Set. However, when I then add another 'Base View', only this time I selecedt the view which was defined automatically when the Flat Pattern was created, a second Component was automatically added to the Master Model Drawing only this time it used the 'Entire Part' Reference Set and everything came out exactly as I wanted it to, and I didn't have to change any setting or switch Reference Sets. If you just let the system do what it wants, you will generally get what you need to do the job correctly.

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.

 

[hudson888]

moog2,

Make sure you follow John's earlier instructions absolutely to the letter, and don't confuse "flat pattern" with "flat solid".

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[moog2]

I've tried to follow his reply, flat solid is what i meant, not flat pattern, but this doesn't get added to the model ref set?
John says "with the Solid in the Model Reference Set",
Does he mean i should add the flat solid to the model ref set?
Also he says, change the " view to the one which was created when the Flat Pattern was defined ",
Does he mean a view should automatically be created when i create the flat solid?
I'm having trouble understanding the purpose of the system created "flat solid" ref set...
The drwg can only see one ref set, therefore it can only draw, the formed OR flattened part??
Unless i add the both features to a new ref set,
John seems to be explaining how this can be done from the std model ref set How??

 

[BOPdesigner]

In the case of the Flat Solid, what I do is in the drawing file, after creating views of the formed SM part, I copy and paste a 2nd instance of the component and switch the reference set of that pasted copy to the FLAT_SOLID. Then I move that component to a different layer, and use Visible in View on the drawing sheet views to set up the view(s) with the flat solid only.

 

[moog2]

Aaahhh ,its all clear now, Johns mathod work fine from "flat pattern", i was using "flat solid", i new it couldn't be THAT hard.
BOP, comprendez, i was just trying to avoid these extra steps, but it's actually not that bad eh?