Pro/Report and Simplified Reps and exploded view - Urgent Help

[texaspete]

First, I have a final assembly that has a simplified rep name rep0001. The rep only shows all the plastic parts of the final assembly - every thing else is excluded from the rep. approximate 24 parts showing from 146. now lets talk exploded view - I have created an exploded view - nothing fansy just exploded. Now lets talk drawing, I have created one view - an exploded view (same one mentioned above). Now lets talk Pro/report. I have a BOM that currently reports all the parts in the final assembly. My goal is only report those that are present / showing in the Simplified Rep. I noted in the Create>table>repeat region> modl / rep, that I can use it some how. Can someone help me create a BOM that only report a simplified rep. Thanks Texaspete

 

[Hora]

Tex,

It's simple this one. Create your BOM table (or just the repeat region) AFTER you put the simplified view in the drawing.

-Hora

 

[texaspete]

Hora, What do I put in the repeat region. Ex. &asm.mbl.name
dave.maloy@curious-id.com

 

[Hora]

Tex,

You must create the repeat region AFTER you put and set the simplified rep view in your drawing. In this way you'll have the link between your BOM and the view. This is what is missing in your drawing.

Then you can add the text:
&rpt.index| &rpt.qty| &asm.mbr.name| etc etc

There are no special parameters for the simplified reps. You need only to link the BOM with the simlified assy.

-Hora

 

[texaspete]

Thanks Hora, I will try this immediately and post my results. Later Dude.

 

[texaspete]

Hora, I almost have it. The BOM show 30 parts while the actual is 24. The Automated BOM is picking / finds links to 6 other parts, ex, Fan Motor, Torque Master Hinge, Screw. If I looking at the Assembly (.asm) file and turn on the simplified Rep "Moldable_parts_only". The is showing the correct data / info. I must be missing something in your last post
I add the text:
&rpt.index| &rpt.qty| &asm.mbr.name| , just like you have it and it working - almost, Do you have any insight.
Thanks Texaspete - Ps, I will be here Friday.

 

[Hora]

Hi Texaspete,

I think I found your problem. If you have ProE2001, then go to VIEWS->DWG MODE->Set/Add Rep and choose the simplified rep you want to apply the BOM. Then erase the repeat region and recreate it. This shoul work for you. Keep me in touch.

For Wildfire should be similar.

-Hora

 

[texaspete]

Hora, you are right I forgot to mention that I was on 2001. I also fail to mention that I have multiply levels of subassemblies. I learned that after the BOM is create with the Simplified Rep applied to both "repeat region> mdl / rep" and the Simplified Rep applied to the view. The BOM , using your "&rpt.index| &rpt.qty| &asm.mbr.name| etc etc" Ballon the view correctly. On some parts it balloon twice which I removed by "Filter> removed by item" and the drawing / BOM slowing developed to want my tooling agent wanted - a Drawing, ballooned with BOM, and only showing moldable parts. This drawing is very hand and all I have to do is create and applied Simplified Reps to views and BOM Region(s). Thanks for your help. Texaspete

 

[Hora]

Hi Tex,

Keep in mind that repeat region are linked with the default model. If you have several models (assemblies) or simplified reps, make the one you want to add the ballons default, and then create the repeat region in your table. You can have multiple BOM tables linked to each assy/simplied reps.

Good luck.
-Hora