Inventor BOM

[Anonymous]

I am wondering if there is a way of showing same identical items separately on the BOM. for example, I have 2 nozzles on the ASME Vessel and want to give it two different call-out like 5A and 5B to match with the asme caculation requirement. Can this be done? I had tried everything I can think of but unsucessful.

Thanks you all for looking into it.

[Cadmanto]

Did you try creating iparts?  Making two seperate parts from the same factory then inserting each into your assembly?

[johnsonshiue]

I am not sure if this will help. Actually,y ou can have two different components having the same Part Number but listed separately on the BOM table. On the table, you just need to click on "Part Number Row Merge Settings" -> uncheck "Enable Row Merge."

You still need to have two separate parts though. It cannot be the same part with two different Part Numbers.

Thanks!

[Anonymous]

The idea has cross my mind but extra works and time will be adding to the project when you are having quite a few connection on the vessels to be listed separately. I am just curious why Inventor has the option to merge items but not having an option to list them separately even if they are the same file.

[johnsonshiue]

Hi! Indeed, if Inventor BOM would support occurence-based entry, it will solve this issue. Unfortunately, Inventor BOM is component document based, meaning each entry is supposed to be unique.

To support your workflow, BOM will have to treat occurrences differently. For example, you have a part called Bracket.ipt. There are two Brackets in an assembly: Bracket:1 and Bracket:2. In current BOM, the two are listed in one row. Let's say we can list them separately, the information will have to be saved in the assembly and for the assembly only. If the Bracket.ipt is placed in another assembly, you will have to redo what you did in the first assembly.

I don't think it is not doable but it can be tricky.

Thanks!

[Cadmanto]

In the assembly you can promote or demote subassemblies to make your BOM look the way you want as well.

[Anonymous]

Demoting it will give the same result. It does not give you a separate for each of those items.

[Anonymous]

A quick "work-around" maybe is to create a Custom Part within the Parts List for Item 5B and change the existing Item 5 to Item 5A. Then in your drawing, to identify the virtual part, you would select the Balloon function and choose the item you want to balloon. Prior to placing the balloon, right-mouse click and select "custom/virtual". Continue by placing the balloon on the drawing then RC again and select "Continue". A list of all your custom parts will display and allow you to check the box next to the one you desire. (the box appears at the start of each row).

[Anonymous]

Thank you though. Doing that, I will have to change QTY of the original part and I would rather not do it. We tend to reuse alot of common design and you know how it is when you are in a hurry, you tend to overlook the BOM with the assumption everything on the drawing is matched with the model. I ran into a few situations in the past and thank god that was not a costly mistakes.  I just like to see inventor can give you an option for something like this, it already has the other way of merging and why not the other way around.

[bobvdd]

I don't think you need to change the QTy of the original part.

It is sufficient to set the QTY of the custom parts that you add to 0 as explained in image below.

Bob