Is there any way to indentify parts so that they do not show up on the BOM in CREO Paremetric 3.0?

[jforsyth]

We are new to CREO Parametric 3.0.  We are making assemblies and drawings where 75% of the parts are reference parts and should not be on the BOM in the drawing,

Is there any method of identifying these reference parts so that they will not be included in the BOM?

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[mender]

The usual mechanism for not including a class of part is Table>Repeat Region>Filters.  For instance, if you had a parameter 'refpart' which is set to Yes in reference parts and No in regular parts, you could add a filter on asm.mbr.refpart (note you do not need to have this parameter in a column of the table).

How exactly you care to identify the parts is up to your company's processes.

[dschenken]

I have had good luck assigning item numbers to components in assemblies. It is easy to filter out the ones that aren't assigned an item number. Instead of rpt.index, use asm.mbr.cparam.item_number (item_number is the component parameter and could be any name you like.)

I think PTC is working this into WC11 so that the item numbers can be assigned and managed there.

[danderson]

I'm curious why the components in the assembly shouldn'tbe in the BOM?

Are they convenience files for making the assembly look correct or to support assembly  motion?

Examples that i can think of are hose fittings that need to be crimped during assembly, hose routing, rivets, shrink wrap, weld joints, hydrualic cylinders,  parts with press fits, hose from bulk hose, sheet metal flat states and etc.  With the introduction of being able to make parts flexible at the assembly level after you assemble them and using mechanism for moving parts along with parameters, relations, and pro/program at the part level. I now find it is very rare that I need to create a extra part for the assembled state of the assembly and need very few family tables now.

With our assembly model tree driving mfg requirements, extra components are not allowed for released drawings.

Just curious.

Thanks,

Don Anderson

[MartinHanak]

Hi,

how did you get a BOM ? Do you use Bill of Materials button in Assembly mode -OR- do you create table with Repeat region on drawings ?

MH

[jforsyth]

I will try to explain in more depth.

We install equipment on commercial aircraft (Boeing and Airbus).

In our assemblies we show the Aircraft frames, stringers, floors, floorbeams, etc.  Thes are in their own unique sub-assemblies.

These are the parts we don't want to be displayed in our BOMs.

We then create sub-assemblies that contain the equipment that we are installing.  This includes standard hardware, brackets we design, connectors, the different electrical equpment that we manufacture and various misc, parts.  These are the parts we want to show in our BOMs.

As far as the BOM, we are creating tables and using the Repeat Region capabilities inorder to populate our BOMS.

In the parts the awe want to show in our BOMs we have user defined parameters that contain the information that we want in our BOMS.

These parameters are:

PART_NO = the part number (i.e. NAS1802-3-10 for a standard scrwew).

DESCRIPTION = the description of the part (i,e, SCREW, HEX HEAD, NO. 10).

NOTES = this is the vendor or spec information (i.e. NAS SPEC).

These parameters are filled out automatically from our acceptable parts usage database at my company.

The repeat region maps the different parametrers to the correct column in the BOM, along with the CREO parameters of rpt.qty and rpt.index.

In other CAD systems that we have used we could take the Assemblies that contain the REF parts (Airframe structure) and select a property for that Assembliy and indicate to "do not use this assembly or the parts within in the BOM", or words to that effect.

The Assemblies that contain the parts we want to see in our BOMs would have the same property to indicate "use thes parts in the BOM", or words to that effect.

I am trying to replicate this process in CREO 3.0.

I like the idea of the fileter in the Repeat Region that Matthew indicated above.

However, being new to CREO I am not sure how to create and apply the filter.

Some more detail assistance would be helpful.

Thanks for all replies.

[dschenken]

Here's the help on using Filters http://support.ptc.com/help/creo/creo_pma/usascii/#page/detail%2FAbout_Adding_Filters.html%23

Note that filters don't have relations - just one-line comparisons. And they are cumulative; logic errors will tend to eliminate all items.

If you need a relation to evaluate then you can add it to the repeat region relations and refer to the result in the filter.

The place your case runs afoul of the way Creo works is that you are expecting to differentiate un-rolled BOMs based on some level of assembly. I am assuming if a screw is used in a Ref assembly several levels down it should not be lumped in with another instance of the same screw in a different subassembly.

This would not be a problem if there were only Ref assemblies and all the top level parts were assembled at the top level. Trivial.

The problem is there is no obvious property available to the repeat region to distinguish which almost-top assembly a part is included in and therefore determine if that almost-top assembly is Ref or not.

I don't know that it cannot be done, but I'm pressed to think of it. AFAIK the region evaluates each applicable item in isolation. It has access to a lot of information about each item, but it doesn't know anything about an item's relation to any other item. It can be told to look only at the top level, or at all levels, and to group by level if applicable, but it can't collate and group by level simultaneously so if filtering by level would work it would not collate. Maybe that would be what you want.

Filter by item isn't guaranteed to work because it will eliminate any items used in multiple places, no matter if some are Ref and some are not, but that also really just applies to collation, which may not matter to you.

[tmorishita]

An easy way to not show components in the BOM is to select Filters in the repeat region, select  By item, select Exclude , then pick the item in the BOM you do not want to show. If you have fixed the index prior to doing this, you will need to unfix the number of the excluded component (unfix, index), and renumber the BOM

[llie · Accepted solution]

If the part numbers are always changing then I would follow Tim's advice. It is simple and easy to do on any one of your drawings.