Single item line in BOM with quantity >1 but with completely different geometry

[Patriot_1776]

Creo 8:

In an assembly, we're using a 40" flexible bellows vacuum line multiple times (3), but since it needs to be a single item line with the correct quantity of 3, it obviously can't be 3 separate parts.  Yes, I could be sloppy and make 3 different parts but with the part number and description parameters the same, but that's not acceptable because it would make 3 different item #'s.

It's not like bulk wire or tubing etc. where I could simply have a quantity of "AR", these are specific 40" bellows.

Is there a simple way to do this?  I was thinking it "might" be possible using multiple bodies, but we don't want to do that because our Windchill guys say multi bodies cause Windchill issues, plus I'm not an expert in using multiple bodies in Creo (used it quite a bit in NX 8.5 about 7 years ago though).

Thoughts?

[pausob]

No pun intended, but really it sounds like you could use a flexible model to define these flexible bellows vacuum lines...  The varied items are the sweep features that define the 3 variants (in each instance, one is active, other two are suppressed).

[Patriot_1776]

Forgot about the suppression thing in flexible, so thanks for reminding me.....but just tried it and the routings failed.

[kdirth]

What is causing the failure?  I know that having multiple sweeps that intersect can cause failures.  You may need to only have one active at a time, saving it with one unsuppressed and using flexibility to turn each one on and off as needed.

[Patriot_1776]

Not sure, none of the 3 routes worked, and none of them intersected, there was zero reason I saw for the failure.  The flexibility/suppressed features themselves were the failure.  Generally you can intersect sweeps (or protrusions etc.) with zero issues, Creo doesn't care if one solid is buried in another, it just merges them.

Even though I've never personally had to do this before (I'd always had to route bulk wire or tubing and can just make that a bulk qty "AR" part), I'd imagine this would be a common problem.  I'm just doing it for the first time because I'm working on a type of assembly and using different parts than I'd ever worked on/with before.

Yes, I could fudge the BOM and take 2 of the 3 lines out and manually change the qty to "3" instead of "AR" but that's sloppy and non-parametric, and in any case I couldn't add ref balloons to them.  We use quantity balloons and I want to have the qty ballon pointing to one route, and the ref balloons pointing to the other 2.

I was thinking someone else may have run into this before since I know it's too much to ask for PTC to actually have a solution since they're happy to let us beta test everything for them.🤣

[pausob]

I tried the method with this toy model and seems to do what you need:

Not sure what you mean by failed routings - maybe that is an issue specific to the piping module, and it disallows using flexible components?

[Patriot_1776]

I'm having to use references from multiple different parts at the assembly as "start" and "finish", the routes didn't like being suppressed at the assy level via flexibility.

I'm not using the piping module, these are going to be normal COTS parts (stolen from "Robbie The Robot" - LOL) routed manually.  And while it would be fun to model the bellows, I'm just going to show it as a tube since there's a time crunch.

Are those balloons parametric and you just split the quantity?

[pausob]

Yes, split balloons.  The components were just thrown into the assembly "by coincident coordinate system", so placement didn't rely on any other features in the flexible model other than its default CS0.

[Patriot_1776]

Maybe that's why mine failed then when I tried that method, because I need to reference other parts in the assembly for start and finish endpoints for the routing.

[AH_10565398]

Could you cheat it by assembly -> Including two additional copies of the first one, and then just hiding the other two in the repeat region of your bom?

[Patriot_1776]

No.  The BOM would then only show a quantity of 1.  I need it to show the proper quantity.  I'll put the BOM balloon on one of them showing the quantity, and the others as ref balloons.

[KenFarley]

I have a dirty trick for this that may be considered heretical.

I assemble the proper quantity of the "original" part, the one that is properly configured for one of your positions.

Just add the other two in, probably best if they're assembled so their flanges are conveniently located for a balloon to attach. They're just being used so the count comes out right.

On the other two properly configured tubes, make sure they don't have any of the parameters necessary for the BOM to pick them up. They're only being used for visuals. In essence they're being ignored by the Bill of Materials.

Once you've got all the tubes in (one with correct geometry and parameters, two with correct geometry and no parameters, two with incorrect geometry but correct parameters) the assembly, define a view that'll be used for the BOM. Add the balloons. Now, blank the two tubes that have the right parameters but the wrong geometry. Now you have the correct count, and the parts look good.

I know, this is kind of convoluted, but it gets the views you want. I've used this kind of shenanigans when I have items that are embedded within an assembly that I don't want to screw up my hidden line renderings. Once the BOM has the components counted, I can "component blank" them and they'll still be counted.

[Patriot_1776]

'Sup Ken!

I thought about that, but I was looking for a clean way to do it.  Time crunch, so, I'll probably just fudge something...

[jvadalia-2]

Are you using "description" parameter in all parts?

If yes, then instead of Part Name as first column, use asm.mbr.description in first column after Sr. No.

And most importantly use same strings in description for all bellow parts.

This approach will serve your purpose of BOM with exact quantity, even for multiple parts, as "description" will be the main identifier in BOM.

Regards,

Jignesh

[Patriot_1776]

Not sure you understand the issue.  This is a COTS part that is used, say, 3 times, but since it is a bellows hose, it's routing/geometry is completely different each time it's used (different vacuum ports).  So, I need to have it show "3" (or if I add a routing, "4") in the BOM, but need to see the different geometry and be able to attach parametric BOM qty and ref balloons to each routing.

[jvadalia-2]

I have understood your question.

First and foremost is 3 different geometries you can achieve through flexibility. If this doesnt work then use 3 different part files.

Even with 3 different parts are there, what you have to do is, keep "description" parameter value in all 3 parts exactly same.

Use below repeat region BOM table format. Don't use Part name in description.

Sr. No.	Description	Qty.
rpt.index	asm.mbr.description	rpt.qty

I think with this workaround you can achieve what you want.

Only thing you have to take care is you have to fill description parameter value. Don't keep it empty in any parts.

I have used it in one of the project.

Regards,

Jignesh.

[Patriot_1776 · Accepted solution]

Flexible geometry failed.  The routings are too complicated, it's not anywhere as simple s changing a length or suppressing the feature.

Our BOMS are already made, I cannot change them to suit one particular instance.  But thanks for the post!

I'm going to fudge it and move on.

[kdirth]

Check out my reply and uploaded file to this thread from a year ago:

Flexible hose for Reuse in multiple different asse... - PTC Community