Autodesk Inventor BOM for parts with same part number and description but different material

[20031995]

In Autodesk Inventor I have some customized content center fasteners. Original fasteners from the content center do not have a specific material assigned such as A2-70, A4-70, 8.8, etc. So this is why I have created copies from existing bolts, washers, nuts and others from the existing ones, but just changing the materials to my customized materials. When creating a parts list the information that I want to display is the following: REFERENCE, QUANTITY, CODE, DESCRIPTION and MATERIAL. I don't want the material to appear nor on CODE neither on DESCRIPTION columns, because the MATERIAL column is there for display this information. The problem comes due to, for example, two DIN934 nuts of the same size but different materials have the same code (part number) and the same description, and Inventor does not make the difference and just puts *various* at the material column.

[CCarreiras]

Hi!

Different part, different Part Number.... there's no other way.

If there's a different material, it's a different part... despite the same geometry.

[20031995]

Then I understand I have no other option than adding the material as a suffix to the part number, right?

[CCarreiras · Accepted solution]

Yes... something like that... suffix, prefix, ABC,.... something that distinguish the different parts regarding the part number.

BOM uses the part number to create the BOM list, so you cant use other iProperties or parameter to create a separated part list member.

[RajSchmidt]

May I ask why you use the same part number for different parts? As I understand part numbers, they are used downstream to manage manufacturing and purchasing. So, if you have the same number for different nuts, how do the people in purchasing know what to order?

[20031995]

In our ERP software we have all this types of parts coded as you say, with the suffix referring to the material. It is just a cosmetic issue, that I don't like to get a parts list with a CODE column saying "DIN934 M16 - A2-70" and then also another column called MATERIAL showing again "A2-70".

[RajSchmidt]

Okay, so you have that covered, good.

BTW, are you talking about the parts list on drawings or the BOM in the assembly file?

If it’s the parts lists, maybe you could try to get rid of them in the long run and pull the information directly from the ERP?

[20031995]

There's 0 connection between Inventor and ERP, so any problem with purchasing, etc. It's just at the moment of making general arrangement drawings of assemblies with parts lists in them. It is just that I don't like to repeat information, "don't beat a dead horse", you know?

[RajSchmidt]

I see. Mine was just a suggestion for the future. Many of our customers are already working this way: Creating the basic BOM in Inventor, pushing that information to EDM (e.g. Vault). In there you can modify the BOM if you need to and then transfer it to ERP.

Sure, it is quite an invest in technology, but there are also many benefits: You save time and avoid transfer errors.

[mslosar]

It comes down to your part numbering system I would say.

Materials can have widely varying name lengths: 310, A2 70, INC 800HT, HAYNES 160, etc. Not all systems can take a 10 digit extension at the end of a part number of the material. So, perhaps creating a table where everything is condensed to 2, 3, or 4 characters as a material table might be beneficial both ways. 

[b_hufkens]

I don't know if this could help with your specific case or if you still require help. But if I understand, the issue is that you have different bolts with same part numbers but different descriptions and materials etc. And they merge in the partslist on drawings or BOM viewer? If you have for example 5x stainless screw with part number 1.2.6 and 5x steel screw with the same part number 1.2.6. Standard it will show up as "10x - 1.2.6 - varies" like image below? 

If so you can seperate them in your partslist by going to the "manage" tab in your assembly.

Select "bill of materials".

Then on top there is a button called "part number row merge settings".

In there you can either completely disable the merging of components based on part number. Or you can just add those that need to be excluded from this rule.

If you add 1.2.6 to the exclusion list, both will show up as separate items in the partslist.

They now should show as "5x - 1.2.6 - Stainless" and "5x - 1.2.6 - Steel"