Controlling referenced sub assemblies in Top level

If you follow this discussion about 1/2 part in a B.O.M., you could follow the same logic but instead of using 0.5 for the value, you could use REF or something like that.

http://communities.ptc.com/thread/38050

As for is showing up as a duplicate in the assembly drawing, you could make a family table of this assembly with one instance having the parts so that the other componenets are not "floating in space" for your drawings and another instance with these items removed.

Thanks, Dale

It sounds like you have a "parts kit" as a subassembly that needs the components in the right location for a specific top level or next level assembly.

Why not assemble the components into the next level assembly; add the empty subassembly part; (both fully constrained); and drag the components in the next level assembly into the subassembly in the model tree. it becomes a restructure function but it should maintain the next level assembly references.

Of course, there will be external references on the subassembly. The plus side is that this will maintain associativity as long as the next level assembly is open when the subassembly is opened.

I understand that you do not want to modify your models and just find an easy way to show some of the parts from top assembly on the drawing, right?

If you do not want to modify your existing models, you may try external simplified reps.

They allow to remove, but also to add parts as needed for an alternate representation - which is basically what you want to show in the drawing.

See for example this thread about External Simplified Rep: http://communities.ptc.com/message/251572#251572

Another method is adding the top assembly to the view and blank the components you don't need. The good old Component Display function is still there. It allows to blank and unblank subassemblies and parts.

So you can blank the whole subassembly and then unblank single parts to make visible again.

Of course you can use layers as well for blanking.

In your hydraulics module, I would use a "copy geom" feature to copy in the geometry you need from the top assembly. The "copy geom" feature will create surface copies of other parts. They can be assigned to a layer so that they're not visible. And they won't show up in the BOM since they are features and not components.

I have a similar problem but it involves the BOM on the drawing. I want "reference models" as I call them to be automatically filtered in the BOM (without having to filter the BOM table) AND have the ability in Windchill to show the BOM only - not the whole document tree.

FYI - everything we want is brain-dead simple in SolidWorks. You can RMB click on the model tree and there are settings for 'Include In BOM", "Include Children in BOM", and "Show When inserting assembly" or something like that. They have all the bases covered to my experience. With these 3 things you can

1) Show only top level assembly in BOM

2) Show only children and skip top level assembly in BOM

3) "Hide" some parts when inserted in a higher level assembly

These settings are carried on the "link" not the file, so you can change them on a "per usage" basis.

If someone can help with these problems (without having to restructure Winchill or write macros) let me know.

Vinod,

You actually have an answer in your own mail: use Shrinkwrap Feature in pipinh / harness assembly to capture all required references form any required level of top assembly. Thisis exact reason why shrinkwrap feature was created for. You can control its dependency i.e. you can "freeze" it for a while, or keep associative to top assembly.

IN your piping / harness assembly, first thing create this shrinkrap feature. Use Subset to only include relevant external models in it. This is very powerful feature with many options. BY default it will collect solid surfaces of components in subset, so if you need datums - add them manually.

Now create your piping / harness and reference ONLY to this SW feature.

Next time you get your piping / harness assembly you will see that shape of reference modules, but you will not have them neither physically nor in BOM.

In top assembly, if surfaces of this SW feature make any trouble - just Hide it. If you want to hide it in top assembly but to keep visible in piping / harness assembly you may need to create a special part for this SW feature, and comtrol its visibility from top assembly through layers.

Hope this helps,

- Vlad

Hello Vinod,

have the answers and suggestions helped?

What was your experience with them and how did you finally create the drawing?

If one or more answers in particular have been helpful or "correct" for your needs, please take the time to mark them. This helps other community members to easier identify the answers.

Thanks,

Gunter