Multiple Item Numbers for Similar Parts in Inventor Parts List

[Anonymous]

Hi all,

Inventor groups items by part number for example and gives a total QTY for the item as well as a single “Item Number”.

So for example duplicates of the same part will show in the Parts List under one Item number, showing the QTY of that specific part and then its properties like Part Number or Stock Code etc... So when you Balloon the assembly all the parts that are similar/duplicates will display the item number "1"

Example:

Please add a way to setup the parts list so that it allocates an item number per item that will still get grouped yet still be independent from the others of the same type.

Example Below

And then when Ballooning the parts of the assembly the similar/duplicate parts must have their own individual Item Numbers

I know it can all be changed manually by editing the values and overriding the Balloon Item Value etc... But when you have lots of parts in an Assembly its nice to have it update automatically when parts get added or removed and if you have multiple sheets.

I know that if I put a duplicate of a part in a assembly I can go change the name, Part Number etc to make it its own individual part and it will be displayed separately in the Parts List and given its own Item Number in the Parts List and when it gets ballooned, but my issue with this method is that when I modify the original part the other ones will not adjust accordingly and I can't always rely on modifying the copied parts and adding associative links and projected geometry etc.

Thanks

Wian

[CADMonkey4Life]

In failed searches for finding a way to make this work I now put a suggestion to be added in future releases. Where welding procedures are of high importance to some industries both be able to blace induvidual unique welds but also isolate components to be shown as separate components but grouped by family. This to make sure you have tracking on the correct weld between the correct parts.

So when placing a piping component, a way to enable " unique component tracking" as a BOM alternative would be greate.

[DRoam]

I'm not sure I understand what you're after. So you want all instances of the same part to be grouped together in the BOM? Is that all you're asking for?

[dgorsman]

I think I see.  The intent is to assist with weld mapping when doing piping spools (and in some cases, material control files).  When there are multiples of an object (e.g. the flanges in the provided picture), you want them all tagged as item "1", with sequential individuals as "1.1", "1.2", not as "1" "2" "3" etc.  If the pipe is similarly tagged as "4.1" and "4.2", then weld 1.1 < = > 4.1 can be differentiated from weld 1.2 < = > 4.2.

[CADMonkey4Life]

Right on the money mate. Only way to almost do it now is to add the ex flanges to a sub assy and use legacy grouping in BOM but it's not exactly what I'm after.
Let's hope they come up with something.

//David

[DRoam]

Oh I see, thanks for clarifying for me. That's interesting... so what you need, that Inventor currently can't do, is two things:

1) For each instance of a part to have its own line on the BOM

2) For the Item numbers of those instances to have the 1.1, 1.2, 1.x numbering scheme

Number (1) is definitely not currently possible--sort of. There's one way I can think of that you could make this happen. If there's usually a relatively small number of instances of a single part, what you could do is use the "Save and Replace Component" command, or some other workflow, to make each instance of a part actually be its own part file. This would make each instance have its own line in the BOM (as long as merge-by-part-number is off), and you could assign them unique Item numbers.

For number (2), iLogic might be able to automate this. I'd have to do some experimenting before I could say for sure.

But this definitely would be much simpler if there were built-in functionality for a "per-unique-instance" option for the BOM, as you're suggesting.

[DRoam]

Come to think of it, I think having each instance that you want to differentiate as a separate part file is the ONLY way Inventor could do this, because it's the only way you could specifically give different iProperties to each instance.

Inventor currently has no way to differentiate between different instances of the exact same part file, because each instance of the part file, of course, has the same iProperties--the same Part Number, item number, everything--because they're the same file!

The only way you could differentiate between instances would be to have each instance also be its own part file. I'm guessing that's what you had to do to make the drawing in your picture? Unless I'm completely forgetting something. 

[CADMonkey4Life]

Yeah as for now the workflow is to place the component as custom and giving each (in this case) flange different filenames. Still it generates manual work rearranging the BOM and setting all the Pos nr manually.

[DRoam]

Yes, I see what you mean. This would be nice functionality to have. 

In the meantime, if I could come up with an iLogic rule that would go through the assembly and assign these sequential numbers to each instance of a part, would that be helpful? You would still have to make each instance of a part its own file. If that wouldn't help much I won't bother, but if it would I can look into it.

[CADMonkey4Life]

DDroam,

That would be very kind of you if you find the time and will to do it 🙂 We are currently sorting the BOM automaticly with a prio column that isn't visible so the flanges, pipes, elbows already groups in the BOM. So we are just left with the hassle of renaming the Pos nr *phiu*

[DRoam]

Sure, I'll look into it 🙂 may take some time though, but I'll see what I could do.

One thing I need to know is if the parts you want to number like this are always within a single, one-level assembly, or if they might be within one ore more sub-assemblies?

[CADMonkey4Life]

We always have them in separate assemblys with separate BOM. So short answer yes 😉



David Olsson
Mechanical Design Gothenburg
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[Anonymous]

It becomes especially difficult / complex when you need to differentiate between multiple hydraulic valves (of the same part number) in one assembly that require setting up differently. i.e. one valve might have to be set to 25bar whilst the another to 50bar and both are indicated as Item #1 on the assembly. Could result in quite a bit of confusion in the workshop...

[NachoShaw]

in that instance then, couldn't you just set up the part / as an ipart/iAssembly of the same instance but different versions? That way, you maintain the single 'part/Assembly' structure but can assign different Part numbers etc that are derived from the root.

would make more sense doing it this way and the features already exist

Nacho

[PaulMunford]

Just thinking out loud - could you turn off 'part number merge' in your BOM, and then use grouping in your parts list to give you the result you are after?

[Anonymous]

Hi @PaulMunford,

I have tried this but to no success...

I have played around with every single setting I could find but it still groups all the same parts under a single Item Number...

@NachoShaw,

Thanks for the suggestion, I have not looked into using iParts / iAssembly as I want to stay away from it. A lot of people never make use of iParts and looking to find a solution that would suit them as well. I will however still look into your suggestion just to see if it works, thanks

Kind Regards

Wian

[DRoam]

@Anonymous, to clarify -- all of the instances of a given part ("Tbracket" for example) are the same Part file, correct? You simply want a unique balloon indicator for each instance? So that you can say to your colleague something like: "Tbracket Item 6 got broken out in the field", and they'll know which "Tbracket" you're talking about?

If so, that's why trying Paul's solution didn't work for you. Parts List "Grouping" will only group separate Parts List line items, and currently the only way to get separate line items is to have separate Part files. In other words, you would need each instance of a Part to be its own Part file. Which, for nearly all situations, is impractical.

This has been discussed a little before but didn't get much attention: Unique piping parts parts list. This user needed to do the same thing as you except he wanted to keep each instance (with its unique Item #) on its own Parts List line. But the premise is the same--both of you need the ability for each instance of a Part to be its own "line item" with its own Item #, and one of you (you) would group those into a single line, while the other (CADMonkey4Life) would leave them on separate lines.

So summing up, Inventor needs the new ability to assign an unique Item # to each instance of a Part in an Assembly. And the only way to do that right now is by saving each instance as a unique Part file, which is pretty much unrealistic. So for now, you're kind of screwed, until Autodesk adds that functionality.

That being said... there MIGHT be a way to use iLogic to re-number your BOM's Item #'s, and while doing so, identify if a Part has, say, 3 instances and then assign in the next 3 Item #s separated by commas, then continue. I think that's do-able. The hard part would be then overriding each Balloon label to be the correct number for each instance of each part. It might be possible.... but I'm not sure. But I think that's your only hope for an automated solution at this time.

[PaulMunford]

You're right - Turning off the 'Row Numbers Merge' option doesn't help.

I have found a work around for you to try...

1. Demote Parts into Sub assemblies.

2. Set sub assemblies BOM status to 'Inseparable'.

3. Create a standard field (I used Stock number).

4. Group on the standard Field.

[Anonymous]

Hi guys,

@DRoam - Yes that is basically what I am looking for, think it would be pretty great if Autodesk can add it to Inventor and also the suggestion that (CADMonkey4Life) made. It can all be done manually but it takes so much time and you need to constantly remember any manual changes you made to the parts list and balloons when you start editing your assembly

@PaulMunford - Thanks for the suggestion Paul I will keep this in mind and try to use it in the smaller Assemblies to help simplify the task a bit. I stumbled on to this also this morning and the only consern I have with this is that by demoting the parts into Sub Assemblies I am now creating more files that need to be stored and processed etc. Which is fine on the bigger Machines but for smaller Machines you'd like to keep it as simple as possible.

My last resort is to try iLogic, which isn't really my strong point. 

I worked in the Manufacturing industry for years now and never used iLogic or any iParts/iAssembly's at any of the companies, so would like to find a solution to the problem without using iLogic as I think there is lots of other people also who don't really use it that often

[Ruffy85]

Maybe this is fixed in higher Versions but in 2015 its not possible to split Parts with the same Part Number in the Bill of Material. 

In our Company we need that, because all each of them have unique tags, which we had to add in the Bill of Material on the Drawing. But when Inventor merges everytime all Items with the same Part Number, i have to add for each Item a new Row in the Drawing Partslist to add the Tag for every Component. That hurts!

[PaulMunford]

If you click on the Merged parts in the BOM, and click 'show' - can you perform your edit?