Frame Generator Cut List - Item, Merged, Grouping, Equations, etc.

[SalesBS29V]

Hi all, I'm creating a custom cut list for models made with frame generator & am having trouble with a few values.

• The first being the "Item" column: It's blank for now because I don't want multiple numbers listed in the same row (1, 3, 5, 7, 9) which results when the "display item numbers" box is checked in the grouping menu. I have grouping on for "Part" & "Nominal Length" with the boxes for displaying group participants & display item numbers unchecked for the time being. I've read two posts (below) about adding an equation: =<STOCKNUMBER><MASS> to the Part Number column in the BOM to roll these up but I want my actual part number still displayed there.. How else can I merge the item numbers for identical parts with identical lengths?

https://forums.autodesk.com/t5/inventor-forum/frame-generator-part-list-qty/m-p/1994602/highlight/tr...

https://forums.autodesk.com/t5/inventor-forum/parts-list-amp-bom-amp-stock-number-amp-sheet-metal-ex...

• The second being: My "Cut Length" column for now is pulling the same value as "Nominal Length" however I want certain parts to display that nominal length (G_L) value minus either 1/8", 3/16", or 1/4" depending on their gauge. For now this is entered manually or simply not displayed at all. Where can I add an equation to those certain parts?
• The third being: The precision in the "Total Length" column needs to be 1/16" but when it's changed under "apply units formatting" to anything other than 0, I get a few "Incompatible Units Error" messages. Unsure why.

I've got "enable row merge on part number match" unchecked in order to report different lengths of the same part number. I hope this makes sense, any guidance on these points is appreciated as I keep trying to sort them out!

-Vanessa

(Using Inventor 2021)

[pcrawley]

Hi @SalesBS29V.  I "liked" your post because of the effort you put into it.  If only all posts were this well researched and thought through.

• Part Number Merging: Unfortunately, the BOM editor only gives you the option of merging on Part Numbers. So if you want identical parts merged and counted, you need to match the Part Number iProperty.
  
  If you want to keep the existing Part Number but merge on say =<STOCKNUMBER><MASS>, you'll have to get creative by copying the Part Number into a custom iProp.  Then you can edit the Part Number iProp to be the mergeable data (like my post you found from 11-years ago!).  Remember to update the drawing's Parts List to reflect the new iProperties in use.
  
  
• Cut Length: I think the answer to this is an equation placed in the Content Center template for the appropriate section(s).  If you can give me an example of the section and where you want the changes (1/8, 3/16, 1/4) to occur, I'll see if the iLogic option works.  (I'm thinking something like:  If G_T < x then fraction = 1/8 else fraction = 3/16 etc.  The most logical function for these situations is a Case/Select statement.)
  
  
• Total Length:  This one could get confusing because of the terminology... 
  There are three quantity-related BOM values for Frame Generator parts:  QTY, ITEM QTY, and UNIT QTY.  You use the word "Qty" on your Parts List but it is reading the ITEM QTY value.  I'll stick to the BOM value terminology to avoid confusion:
  
  - ITEM QTY value holds the counter for the number of identical parts.
  - UNIT QTY contains the individual part length.
  - QTY is ITEM QTY multiplied by UNIT QTY to give the total length required to make all the identical parts.  
  
  Did you make the frame, then edit each frame member, and change the units formatting in the parameters table?  If so, is it possible you didn't apply/save the parameter-table edits?  It is also possible (I haven't checked) that when you change the rounding to a fraction, you are changing the property from a "number" to "text" (It's not something you'd click - it's how Inventor handles non-numeric entries).  Therefore, on some parts, you get "0" (number), and on others, you get "3/16" (which is text).  Hence the error.  Can you go decimal?😉
  
  You can edit the Content Center member template to control the default unit formatting to ensure nothing ever get missed - and it'll save a LOT of manual editing!  (You can do it at the same time as adding the iLogic equation mentioned above.)

I know these aren't answers (yet), but I think what you want is achievable with a bit of persistence.  I know from experience that getting the model right (and presenting the correct iProperty data) saves hours manually editing drawings.  If I am right about how you set all the exported parameter formats, then editing the CC template will be your new best friend!

[SalesBS29V]

Wow Peter, who better to respond than you, thank you! Glad to see you're still active here in the forum, sorry I've been busy with a few projects since last week.

• Understood on the part number merging - this would be so easy if there were just another check box! So I've added a "description" column that I want to pull the part number, then I'll hide the merged part number column. I thought the right route was to open the content center editor>family properties>template parameters & add it there (see photo) but the description column for that one test member hasn't populated. 🤔 Do I need to open each .ipt to add that to it's iproperties? 

(I went along on this route & fear some of our content center practices are not the best.. My coworker uses Inventor 2020 while I'm on 2021, we don't use vault but have a folder containing most of our common members that we've used to publish our structural shapes. We both customize & add to these shapes as needed on our separate machines - I simply customize & publish the shapes I need to my content center - without saving over them there to avoid merging them to 2021. Of course in hindsight they should have been copied & saved somewhere, maybe I assumed they were by being a published structural shape? Phew, I think I have some content center overhaul to do to get it right.. been figuring it all out from the start for both of us!)

• For the cut length column, I'm thinking of circumventing ilogic for now by adding a gauge/mils column instead as I don't necessarily have all the separate members to represent them just yet. Still thinking on this. I do want to learn some ilogic soon though, will keep this idea for then.
• For the total length column - "apply units formatting" is applied as the default is in inches. To change the default units & precision for members in the content center, do I need to again open each one, edit  & save it's document settings?

I appreciate your time, help, & reciprocated persistence!

-Vanessa

(Using Inventor 2021)

[SalesBS29V]

Oops, the page had an error, here's that template parameters photo.

-Vanessa

(Using Inventor 2021)

[SalesBS29V]

Update: I have since found the incredibly helpful "open from content center" feature so that I can open, edit, & save copies of my (2021 version) custom members, then replace their family template in the content center editor. Still however having trouble getting my "description" column to display the part number despite editing the member's iProperties.. 🤔 though for non-content center parts this column does update. Maybe I missed a refresh/update button somewhere.

I also found the "custom property format" in each member's parameters to change the default units & precision to 1/16" but when changing my total length column to "use default formatting" they stubbornly remain in inches.. 🤔

Will keep chipping away at this as my time permits.

-Vanessa

(Using Inventor 2021)

[jtylerbc]

@SalesBS29V ,

If you're saying that you are trying to use the actual "Description" iProperty to act as your substitute Part Number, the problem is most likely that the Content Center Family Table is assigning values to the Description field that are overwriting whatever you are trying to put into the Family Template.

I would suggest using a custom iProperty as the substitute for Part Number, instead of trying to use the Description and fighting with the table.  Alternatively, you could remove the Description property column from the table.

[SalesBS29V]

I just found a critical sentence in another thread here.

"After you use the replace family template command only new parts you add will have the additional formatting."

Inconvenient, but okay. A small test model confirmed that is the case.

-Vanessa

(Using Inventor 2021)

[jtylerbc]

Ah, yes.  That would do it also.  Probably should have asked first - I assumed you already knew that, and that you were seeing the problem on newly-placed parts.  

If it was happening on new parts, the table issue I described would be a likely cause.

[pcrawley]

Hi @SalesBS29V 

Looks like I've missed a few posts, so not sure where (if) you are currently stuck.  

I did notice that you are still seeing "inch" units.  That's fixed by:

• Open from Content Center - create a part from the family in question
• Tools > Document Settings > Units - set to metric (don't forget the mass units as well)
• In parameters, I typically set custom units formatting for G_L to 0 decimal places, otherwise, all your length values on parts lists come out rounded to 3 decimal places - and the people in the shop might laugh...
• Replace the family template (of which you are now a fan).

The "Description" is (possibly) easier to define in the Content Centre Editor.  I typically define all my properties here because it's easy to manipulate.  If you have some properties set in the table editor and some in the part template then it can become more complicated to manage long term.