How to get the same part list(BOM list) numbers on individual parts on mono drawing?

[jelle5QCJN]

Hi,

I got a quick question about part list numbers. When I place the part list on a assembled design, inventor places automatically generated numbers to each part. But when I start making my mono drawing with each individual part it gives each part the number 1. How do I solve this?

so my question is, how do I get the same numbers generated on the assembled design on the individual parts without having to manually change the number to the correct number?

I have attached an example.

Kind regards,

Jelle

[Mario.VanWiechen]

We use some Ilogic code to do that. The "Item" number from the BOM is written to the part as a property, " BOMNO" in our case. Your balloon then has to be setup to display that property.

Only complicated the first few times. Grin

[EdvinTailwind]

If you place a new Base View of the whole assembly and then turn off visibility on the parts you don't want show, the remaining parts will still have the correct number. Like this:

[Mario.VanWiechen]

---

@EdvinTailwind wrote:

If you place a new Base View of the whole assembly and then turn off visibility on the parts you don't want show, the remaining parts will still have the correct number. Like this:

---

We used to do that, every separate part had a separate View Rep, what a PITA.

Cant imagine using that method for more than a few parts and would not work on a separate drawing

[EdvinTailwind]

Indeed! Didn't say it was optimal for workflow, but it works and the numbers originate from the BOM, so the link is kept short without any custom Properties. 

And actually, separate View Reps are not needed (which I do see the point of having, but also the amount of extra work). Visibility can be toggled directly from the drawing view tree.

[Frederick_Law]

Give each part a part number and use part number.

Item number changes from assembly to assembly.  Take extra time to manage and maintain.

I had removed Item number in part list  and balloon with Part number in some jobs.

[jelle5QCJN]

Hi thanks all for the quick replies,

@Frederick_Law 

 your solution seems to work nicely indeed, the only trouble is that I got quite long names (e.g. if I would add bolts from the content centre it will say ''ISO 8676 - M8 x 1 x 16'' in the balloon)

Is there a way to change this?

I tried changing the part number of the content centre bolt name in Iproperties. But then I got the following warning

'' Cannot modify the library file C:\Local Workspace\Content Center Files\en-US\ISO 8676(1)\ISO 8676 - M8 x 1 x 16DIN EN.ipt
Component C:\Local Workspace\Content Center Files\en-US\ISO 8676(1)\ISO 8676 - M8 x 1 x 16DIN EN.ipt is not checked out to you. Edits are not allowed on this file.''

 Kind regards,

Jelle

[jelle5QCJN]

Hi thanks all for the quick replies,

@Frederick_Law 

 your solution seems to work nicely indeed, the only trouble is that I got quite long names (e.g. if I would add bolts from the content centre it will say ''ISO 8676 - M8 x 1 x 16'' in the balloon)

Is there a way to change this?

I tried changing the part number of the content centre bolt name in Iproperties. But then I got the following warning

'' Cannot modify the library file C:\Local Workspace\Content Center Files\en-US\ISO 8676(1)\ISO 8676 - M8 x 1 x 16DIN EN.ipt
Component C:\Local Workspace\Content Center Files\en-US\ISO 8676(1)\ISO 8676 - M8 x 1 x 16DIN EN.ipt is not checked out to you. Edits are not allowed on this file.''

 Kind regards,

Jelle

[cadman777]

I do it similar to @Frederick_Law, by creating a Custom iProperty specifically for numbering parts.

Then I went to the Inventor Customization forum and found some code that pushes that iProperty from the Assembly BOM into each individual part, and then into the single part ViewLabel.

It took a lot of work to figure out how to get this done b/c I suck at iLogic/VBA. It also took a LOT of help from the experts in the Customization forum. But at least it works good enough to get the job done.

If memory serves, I have 6 different iLogic 'rules' cobbled together using a VBA 'macro' to make this work. What a PITA for something that should be integral to inventor! Especially b/c Numbering is one of the most important steps in a design/engineering project.

Incidentally, my 'rule' also adds the TotalQuantity to the single part view label (which was even more difficult due to the way Inventor handles part quantities(!).

So my advice to you is to create your own Custom iProperty specifically for single part numbering, KEEP IT SIMPLE, and go to the Inventor Customization forum for help in accomplishing this.

[Frederick_Law]

For Content Center, copy the one you use and change Part Number to what you want.

Not a simple task.

Copy and make it custom library.  Right click on the column title to edit how to format the column.

I copied Heavy Hex Bolt to "make" ASTM A325 HEX just for BOM.

You can delete size you don't use or add missing size in this custom library.

[NigelHay]

If you insert your screw into your assembly then R.Click on it & select Properties, Project, you can see that the Part Number defaults to the file name (ISO 8676 - M8 x 1 x 16). We do what has been suggested here, save it using the numbering convention you want. If you do this as you go along, you will quickly build up a library of parts numbered the way you want.

[cadman777 · Accepted solution]

What this boils down to is you have to do some Customizations to Inventor.

I do a similar thing as @Frederick_Law.

1. First create a CustomLibrary of each category you want to change.

2. Then open one part in that category and add the new iProperty (I call it MARK')

3. Leave it blank or type in the formula you want.

4. Then save that part file and Replace the FamilyTable Template file with that part.

5. Then add a column with the new iProperty to your PartsList in your drawing Template.

6. Also add that same iProperty column to the BOM in your assembly Template.

I think that's all you need to do to be set-up for the future. Any new categories of parts you can do the same thing, except you don't have to add a new column to your BOM and PartsList b/c it's already there from the first go-around.

Incidentally, I leave the MARK blank till it's time to number parts. Then I go to the BOM and sort all the parts so they end up in categories by shape, size and dimensional description (most often 'Length'). Then I use Inventor's built-in BOM automatic numbering. If there are parts that I don't want to renumber, then before auto-numbering you can Lock them. Then after they are numbered, I copy that entire column and past it into the MARK column. Then Numbering is finished. You can use your iLogic rule to reference the iProperty named MARK (or whatever you name it) and send the value anywhere you want in the drawing. 

[rhasell]

Hey Chris

Apologies for hijacking the thread, ;(

Are you able to do total quantity with model states? My code is filename based, so model states fail to count correctly.

Thanks.

As for the item number issue, I use a custom property based on project name/number.

Copy the GA item number to the custom property. This property be used for labels, balloons and BOM. (Library parts are ignored, due to RO property, in my case, not a problem, actually preferred)

[jelle5QCJN]

Thanks, for the detailed steps. How do I create this new iProperty, that you describe in step 2.? I am a bit lost..

Kind regards,

Jelle

[cadman777]

Let me warn you that there is a bit of a learning curve to this, but it's not too difficult.

First you must create a Custom Library so you can edit your CC parts, which is a separate process.

Then you find the part you wan to edit and RMB on it and select FamilyTable.

Then you have to learn how to use the FamilyTable.

It's real easy once you learn the various parts of it.

YouTube has some real good videos to learn from. 

[cadman777]

Hey Reg,

I don't have ModelStates in my version of Inventor.

Everything I do is ancient!

Sorry I can't be of any help.