Content Centre Part Number Expression

[gcoombridge]

Hey everyone...

I've made a structural section for frame generator following Autodesk instructions (and also a word document put up by a forum user). Basically I'm dealing with structural stainless sections with unusual dimensions and wanted a more concise description/stock #. i.e. SHS, 25 x 3, SS 304

I've made the base part, published to content centre and altered the parts number expression to: {Member} & "-"  & {B_L}

I want it to be: SHS, 25 x 3, SS 304 - 500mm (for example)

I get this error message:

When I create a frame the part number only contains the static value of B_L in the BOM! Base QTY and Item QTY display properly.

This problem seems to be in the content center end but I'm not experience enough with this to be sure... Anyway I'm visibly aging by the hour so if anyone can help that would be much appreciated! I'm using Inventor 2017

I'm doing something wrong somewhere I guess..

Thanks

[Mark.Lancaster]

@gcoombridge

A couple of things...

Read the message again: ..   The issue is related to the file name column.  Each member must have a unique file name  and it appears you don't.  Make sure the file name column expression has the length value added as well.  In addition Inventor 2017 had issues with content center..  So make sure you have all the latest updates that you're entitled to..  Report back on your progress.

Update:  Also your length (B_L) column..  The cell values are black..  Which means they are static and not compliant with the custom expression you made.  Highlight all of them in that column, delete and they should turn to back to blue...

Update #2: That holds true with any other column that has an expression assigned to it.  The column cell values must be shown in blue in order to be linked to the expression.  If the cell value is black than its a static value.  Update you family table as needed because your images are showing that all the cell values are black and static.

[gcoombridge]

Hi Mark,

Thanks for your help..

As for the software update I will check that shortly...

The filename does include the B_L expression (see pic)

 The B_L column will not allow me to remove the values..

Thanks

[Mark.Lancaster]

@gcoombridge

But the cell values are black which means they are static..  So Inventor is not seeing unique file names.  Yes you have an expression there but each row/each custom length will always have the same file name.   You need to reset each cell value by highlighting the cell value, delete it and it should go back to blue (and then it will be under the control of the column expression)

Here's an article for your reference:

https://www.synergis.com/2014/02/28/working-with-inventor-content-center-part-1-of-3/

https://www.synergis.com/2014/03/17/working-with-autodesk-inventor-content-center-part-2-of-3/

https://www.synergis.com/2014/03/28/working-with-autodesk-inventor-content-center-part-3-of-3/

  It talks about the colors of the cells/column headers and few other things.  Use it as reference material and also in that article is the link to part 1 and 2 as well.

Any other questions please let us know or private message me.   But you need to get your cell value colors back to blue..  You may want to just do 1 cell at a time..

Good luck.. 

[blandb · Accepted solution]

Just a thought, if you have to do something like this again, you could of found a structural section that was very similar to what you want, or the EXACT one that you want, but with a different description. To keep from modeling the entire part from scratch, you could of just did a "save as" or copy to your custom read-write library, then just altered the family table. All the hard work would have been done for you.  The reason I say this is because you stated that "you published" your new part. I just wanted to make sure you are aware that you can copy existing families and then make them your own.

Hope this helps for next time!

[cbenner]

@gcoombridge

What expression is in your B_L column?  Is it a range expression? Like:

Also... in Frame Generator, the file names of frame members are generated by the program from Stock Number and an auto generated unique number.  What you have in the File Name column in Content Center is not what you get from FG.  If you placed a piece of that steel just by itself without the Frame Generator (Place from Content Center) do you get the correct file name?

[gcoombridge]

Mark - The values in the B_L column are black but cannot be edited, I understand what you mean but when I select and hit delete I get the pictured error message (invalid cell value).

I decided to take your advice and adjust a copied family. Interestingly as soon as I changed the material drop down from mild steel to stainless steel the B_L column went static (blue to black) on the copied library. I updated to 2017 R3 and it worked correctly. Unfortunately the problem with my authored library persisted.

Work wise I'm sorted but I am curious about why my authored library does not work. Thanks for the article, very helpful in understanding how the system works.

Chris - the range is set to 0.001;200000. I'm not too worried about the file name as long as it meets requirements. I like to have itemized cut lists on idw's. For this I need a unique part number for each material and cut length combination otherwise they group together. I have been using the description to describe the material and base qty to give cut length.

Thanks again - I will play a bit more but it may be to do with the way I set up the parameters in the base file I guess..

[gregory_nickol]

I know this thread was last active 7 years ago, but I came across it while searching for something else. In regards to the "Invalid Value" error when trying to delete a static value from a cell that is set to custom. The reason is that the cell range is set to a minimum of something greater than 0 such as 0.01 or 0.001, and deleting the active value treats the cell as a 0, much like a blank is calculated as 0 in an Excel formula. Two potential workarounds:

1) Change your expression to minimum of 0, then delete values as required, and change back if worried that 0 will cause an issue. 0 Would of course be invalid in that you can't generate a 0 length extrusion and the file will fail to generate, but you don't ever need to make that file just like how you don't ever need to make a 0.001 thick slice of a beam either so it's not really a problem.

2) Alternatively, use the open in Excel command, delete all values that SHOULD be expression driven but currently show up as static, close and save. When it reimports your changes, it reads blank cells as truly blank, not as 0, and correctly assigns the expression value to the cell.