Item number from assembly drawing to part drawing

[Goran.JutrisaR5QUS]

Hi,

I have one problem.

I have assembly drawing in one idw, and every part in its own idw. 

so i dont have usual configuration like one idw drawing for assembly and more sheets for parts.

when i made assembly drawing i put part list in it, and evey part have its own item number.

now i made part drawings in seperate idw, and i would like to get item number from assembly drawing and link it to new part drawing.

how is this possible?

Thanks in advance

[Gabriel_Watson]

Do you mean get the Parts List / BOM table item number from the assembly drawing to use in each part drawing?

[cadman777]

My way of doing this may not be an 'out-of-the-box' solution, but it's worked well for me over the course of many years. There are 5 things to keep in mind when doing it like I do:

1. Don't use the 'Item',

2. Make your own part number from one of the other iProperties or from a User iProperty,

3. Assign all part numbers in the assembly BOM. I usually do this near the end of modeling.

4. Setup your idw so the part number (iProperty) is referenced somewhere in the titleblock text. Every company has their own titleblock and drawing standard, so you have to us whatever is the standard.

5. The 'Part Number' is the only iProperty that Inventor uses to identify SAME parts in the BOM and PartsList. So you can use that to 'RollUp' your idw PartsList. RollUp means all the same parts will combine into one line item in the PartsList. So I reserved the 'Part Number' iProperty for 'RollUp' only. That simplifies my method.

Since my part number is a compound part number I won't explain it to you b/c it can be confusing.

But I will tell you that I use 'Stock Number' as the part number that shows up in the idw PartsList. You just have to rename the PartsList column from 'Stock Number' to whatever you call your part number. Mine is 'MARK', since in the structural steel industry they call the part number a part's "Mark" or "Mark Number". It's the MARK they put on each part so the guys on the construction site can identify it on the drawings.

See attached illustration...

[A.Acheson]

One way is to create a custom iproperty in each part, populate the assembly number in the BOM where each part is exposed for editing and retrieve this iproperty in the drawing. This will work for custom parts only as a standardized/library part will need a new assembly number. 

I think it is best not to track the relationships in this way as it removes flexibility in the design stage later. The design should be tracked from the top down and not bottom up by means of the parts list. But of course it can depend on your tracking needs. 

[Goran.JutrisaR5QUS]

Thanks guys, i understand everything what you wrote, and i am used to worked like this.

But my company migrated to Voult and i would like to automatize as much as possible. 

creating custom property for item number is my back up plan and i am trying to avoid this.

If someone knows how to get default item number from part list from assembly drawing to link it to part in new created idw drawing it would be enlightening 🙂

[Gabriel_Watson]

Most likely this can only be done by exporting the item numbers and iLogic.

[swalton]

By default, Inventor makes the initial Part Number iproperty of a part/assembly file the same as the file name.

In our process part number=.ipt/.iam filename=.ipn filename=.idw filename.  Our Parts Lists on drawings show both the Item number and the Part Number.  The item number on an assembly print is an index number that is only valid on that drawing and has no other use at all.  The Part Number is pulled from the model's Part Number iproperty.

We use the Numbering Scheme tool in Vault Professional to generate filenames/part numbers when the model is saved for the first time.  We also make sure that the drawing filename matches the model filename.  See: https://knowledge.autodesk.com/support/vault-products/learn-explore/caas/CloudHelp/cloudhelp/2019/EN...

[A.Acheson]

@Goran.JutrisaR5QUS 

You are likely best to do this in vault manually. I don't believe there is any iLogic that can do this for drawings automatically as there is a child parent relationship that is only visible through the parent.

1. An iLogic rule could be used to simply inject the number into each drawing file externally of the assembly ,  looking at each drawing file in a folder, figure out if the drawing has a part file or not by either looking at it's contents or by a pattern in the filename then inject the number. So this would be a drawing to drawing information transfer with no link to the drawing or assembly or parts. 

       2. Alternative is to run an iLogic rule in the assembly look at each part if the drawing is named the same as the                  part in a given location (where the part is held), open each drawing and inject the assembly number.