Bom Problem

[jelston]

I have yet another problem with the BOM in Pro/E. I have two parts that are identical as far as purchasing goes, but one part has a cutout and the other does not. How can I list them as the same part on the bom. If I give them the same description but different parts, one of them will not get a balloon. If i make them same description same part, the cutout will be in both and i cannot have this. Any ideas, tricks, etc.

 

[sip]

Do the cutout in assembly?


Sip

 

[jelston]

I need individual drawings.

 

[magneplanar]

Jelston,

Perhaps a simplified report and a family table part is appropriate. You can name the part with the cutout to be the same basic number plus some simple identification for the cutout. Then in the BOM repeat region you show identify the simplified report view that has all the parts you want to have a bom balloon for. Worst case , you add BOM balloon manually for the part that doesn't get one.

cheers,

M

 

[jelston]

Perhaps a simplified report and a family table part is appropriate. You can name the part with the cutout to be the same basic number plus some simple identification for the cutout. Then in the BOM repeat region you show identify the simplified report view that has all the parts you want to have a bom balloon for. Worst case , you add BOM balloon manually for the part that doesn't get one.

I don't want to use different parts even if in a family table because I want to have a cut list of all material used and the quantity of that material. If use a family table, the descriptions of the part can't be the same; if they are neither item will get a balloon. Also, being that the "powers that be" are so erractic in their decision making, i would like to the BOM to be as automatic as possible (cuts down on mistakes).

 

[Guest]

Create the sinlge part with the cutout. In the part create a simplified rep that excludes the cutout. In the assembly create a simplified rep and add the part that has the cutout you want to remove from the model to the list. Set the assembly to master rep and the part to the simplified rep you created at the part level. Here are some images of what I came up with. The the hole was created by subtracting a cylinder from the block. The other cut is an assembly cutset at the part level. The first column of the table is the part name, the second is the index, and the third is the quantity.

 

[jelston]

I know this is probably ancient history to you guys, but i found a better way to do this. Still doesn't make sense to me that i have to go thru all these steps by here goes:


Make a separate parameter (maybe bom_balloon or something) for all the partsof your bomand change the balloons' driving parameter (Table->Bom Balloons->Set Param) to the parameter you created. Now you will have the numbers you want along with the quantity.
Edited by: jelston

 

[jdurston]

We've done a similar thing for years by using PART_NUMBER parameter in all the parts as a standard and driving the ProE repeat region with asm.mbr.PART_NUMBER rather than asm.mbr.name. By default, we set PART_NUMBER = rel_model_name(), but it can be changed in a particular part.


I think it could be done with more sophistication with repeat region relations, but I don't have great depth of knowledge there.


I was going to suggest using Flexible Components, but you're removing the cutout entirely; so, I don't know you could get that to work. If the cutout were different sizes, then yes.


Never tried changing the Bom Balloons' driving parameters before. Something worth looking into. Thanks for the tip.


Good luck,


JD