Suppression of a component feature in only one view

[BOPdesigner]

NX 5.0.5: I have a modeled a flexible printed circuit using NX Sheet Metal. This component is in an assembly model that I will call Assembly B. A drawing is now started (Assembly A) using the master model concept and assembly B is added to the drawing. I want to do an exploded view of the parts, and in this view I want the flexible printed circuit to be flat. How can I do this and not have that component appear flat in the rest of my drawing views?

 

[hudson888]

Under exploded views hide component in view will work if the feature is a component that you just don't want to see.

There is also a way of adding a view as based on a separate part by setting that up with a difference reference set and adding the view from that part. The trick is that when you go back to the drawing in part1 then add a base view and select the "Part" icon in the left hand corner then select part2 and add the view from it.

last but not least the old fashioned way is to create geometry on different layers and manage the layers that are visible in each view so that most views look like the installed and one is in the flattened condition, or vice-versa.

Cheers

Hudson

 

[acciardi]

I think the OP is asking for something a bit different...

He wants to show an assembly component in one view fully regenerated, but in an adjecent view, he would like to show the component with one or more features suppressed.

It's useful for showing the same component in side by side views but at different states, ie, having the final 'unbend' feature in a sheetmetal part suppressed.

I looked for a way to try this a while back but gave up. Pro/e used to have an operation called 'represent' which would allow one to suppress any feature in a part (even if a member of an assembly) by view. The problem was it slowed the drawing update down quite a bit.

Could this be accomplished with Part Families?

 

[BOPdesigner]

Yes acciardi, that is what I am after. The problem is that there are more than just sheet metal features in my component, so my SM flat pattern leaves some of the later extrusions off the component. What I was hoping for is a way to do a suppression by expression in the component that performed something like if parent_assembly = Assembly A then suppress Bend(4) = 1 else 0. (I know that is not correct syntax) Then I would insert the component into Assembly A alongside Assembly B and use layers to or hide component in view to create my views.

 

[hudson888]

For drafting purposes this is commonly done using reference sets as I described. The suppression by expression may work up to a point but I don't know that it is strictly necessary.

Now the description for how to work with a view from another part is likely to be the key to your needs if you're looking to a flat pattern. John Baker suggests using the Solids in the developed and flat states in his recommended method which I think relies on using a similar technique.

Provided that you have the licenses to run it I very much prefer the curve version of a flat pattern under Application>Sheet Metal>Forming/Flattening>Tools>Flat Pattern. I simply create a reference set that includes it for drafting purposes and work with layers on the drawing.

Cheers

Hudson

 

[acciardi]

This might make a good enhancement request - the ability to use different reference sets in a single model drawing. Then one could replace the MODEL reference set with the FLAT_PATTERN one in a given view.

 

[hudson888]

There is justification given by the fact that it works without requiring it to say that it probably won't be a priority. As I said it can be done using view from another part.

 

[BOPdesigner]

I agree about the flat pattern, and I have tried that. The problem is that some of my features are not in sheet metal. I have a sheet metal part sandwiched in between a couple of extrusions. A hybrid flexible printed circuit board with one bend in the center flexible part of the board. When I flatten the part, the rigid parts of the board remain in the formed state instead of staying attached to the SM feature. I suspect that in the future as the Flexible Printed Circuit Design application matures this will be a nonissue. Thanks for your suggestions

 

[hudson888]

Perhaps then I ought to comment that it is good that you added this last piece describing your dilemma, so that I may at least clarify that we're talking about two different things.

Sheet metal parts are designed to be fit for purpose as installed, the flat pattern is an important process stage. Because the bends are always defined NX can use that information to develop the flat pattern.

If you design printed circuits in the flat and seek to wrap them around a corner then you're working in the opposite construction and may struggle. You may have to take the design and transfer parts of it onto the two faces and then join the tracks (preferably in straight lines) around the corner.

Once you have modelled the installed condition then provided that you express the bent corner as a radius then you ought to be able to flatten it back again using the Forming/Flattening tools. Although you probably won't need to bother with doing so.

I don't know what the development expectations to support PCB's may be, but in general NX expects the designer to supply the information needed to create any and all geometry. Wrapping of flat geometry to a formed shape of any contour requires some extra steps that can supply some interesting challenges, so don't be surprised if it remains easier to work with the geometry based on the method I described above.

Either way you wind up with two versions of the model in different files or reference sets as the case may be. Your basic technique for managing the contents of views on drawings would involve using exactly the same options that we described in earlier posts above.

Cheers

Hudson

 

[BOPdesigner]

Currently (NX5) the difference between NX flexible printed circuit and NX SM is that with FPC, you design and locate all of your discrete planer regions in their formed position within the assembly. Then you join them with a Bridge Transition feature consisting of blends and planer regions, last step is to flatten that for export to ECAD. So we would not be designing it in the flattened state and then trying to wrap or bend it afterwards. More tools for FPC are reportedly in the works.

 

[hudson888]

Okay well if you're having any trouble flattening it then I can maybe add that to flat pattern a Sheet Metal part as a solid then you have to have defined the bends as sheet metal bend features. To use the Forming/Flattening method that I described above then you have only to have regular geometry that could be flat patterned. That is to say that as long as the geometry does not contain freeform contoured elements or the corners aren't constrcuted so that they lack bend relief and could never be resolved to a flat pattern, then the program will give you the curves describing that flat pattern.

It is an extra licence but it is quick and easy to run. We prefer to design in what they call chunky solids technique with the hollow as the last feature at the end. This geometry is appreciated by some who find it quicker and easier to create. And you can take unparamaterised geometry from foreign CAD systems. Neither would flatten the solid, but either should work to deliver you of a curve flat pattern.

Maybe this'll help

Hudson