Assembly drawing situation

[CadGuy59]

Hi All,

I'm looking for a good workflow for an NX 12 assembly drawing where I have a component in an assembly that is a flex circuit. I need to show both the flat solid and the folded solid on different drawing sheets but don't want to use a Reference Set that has both due to display issues in Modeling. It would be great if Siemens would allow access to Reference Sets in the Add Base View function in Drafting as that would solve this condition.

Has anyone else found this to be a problem and or found an acceptable workflow to get around the lack of functionality?

Our current workflow is to add the component multiple times but that affects the BOM needlessly.

Thanks,

RJ

 

[CadGuy59]

Thanks, original post updated to state NX 12!

RJ

 

[jerry1423]

Yes, I saw that after I read it again, then removed my post.
You can import into your assembly drawing a view from another part; do you think that would help your situation here ?

Jerry J.
UGV5-NX11

 

[jesseleonard]

Our company deals with this in our Top Assembly drawings when dealing with different reference sets of rivets (manufactured state and a deformed installed state). Our exploded views need the rivets to be shown in their manufactured (unspun/unstaked) state and the rest of the views are usually needing the rivets to be shown in their installed states. The workaround we use to keep our drawings "Up-to-date" and have different reference sets of the same rivet on one drawing, is to implement the "Snapshot" Lock Method for our exploded views. This setting is found within a views configuration settings under the Lock Method dropdown and is usually default at "None." So what we do is, create the exploded view and set our rivets to the Manufactured reference set, update the view, and then lock it via the "Snapshot" Lock Method. We then revert the rivets back to their Installed reference set within the assembly tree and continue to create the rest of the Assembly drawings, having the Lock Method stay default at "None." This will eliminate the "Out-of-Date" callout you usually see on modified drawings. The only downfall is that the Exploded view will not Update to any modeling changes until you go back into it's view settings and set the Lock Method back to "None," update the view, and then reapply the snapshot.

Hopefully this is the solution you are looking for.

- Jesse L.

 

[CadGuy59]

Hi Guys,

Thanks for the feedback. I've already tried the View From Part functionality but that tends to add complexity to the part file that an average user wouldn't understand, IMO. Plus, it still has an issue with eliminating the folded flex in that view to isolate only the flat solid. Again, added complexity for maybe zero ROI?

The Lock Method sounds promising until a non-part owner has to update my drawing with all that done to it. Pretty high overhead perhaps? I'll look into it though to be sure!

RJ

 

[Toost]

Have you tried the NX sheet metal , and - flat pattern on a drawing ? ( master model )
( i have used the NX Sheet Metal application on Flex Circuits, - to handle the flat/folded issue.)
this will use the "View from part" functionality.
which includes that the view from part -part will not be reported in any BOM's.
Neither will the model in "view from part" show in the other views if this is done using the flat pattern feature.

there is a "Flexible Printed Circuit Design" application in NX, which is quite similar to the Sheet Metal Application.


Regards,
Tomas

 

[Dave K]

What about adding a second instance of the model component to the drawing, on a different layer than the first. Then set this component to the 'other' reference set.

By using Layer visible in view, you can determine which reference set, via separate components, is shown in the different views?

-Dave

NX 11, Teamcenter 11

 

[CadGuy59]

Hi All,

More details based on recent feedback:

I'm already using FCP to create and maintain an associative flat solid. No issues with the flat solid at all.

We don't use Master Model concept here and will most likely never do so.

Primary objective is to avoid adding a second instance of the component merely for a drafting purpose.

Thanks,

RJ

 

[3dr]

Reference Sets and Layers in combination with Layer "Visible in View" is the only practical method I know of to support this.
The appearance on the modeling side never bothered me because it has no effect in the assembly.




Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX11, Win 10 Pro