Frame Generator elements: Automatic Part Number

[Vadim-the-Engineer]

Once the frame created with profiles according to skeleton Inventor fills up parts (profiles) iProperties Project tab: Part Number, Stock Number etc. 

Is there a way to see / control data entered and fields filled? Maybe to assign separate places for separate data types? 

The goal is to receive less stuffed Part Number field and set quantity back to units and not the length of the profile.

Thank You in advance!

P.S. In the attached picture of drawing table Description column is actually Part Number column (value substitution)

[jhackney1972 · Accepted solution]

Take a look at the Screencast.  The "Item Qty" parts list property is the count of the components instead of the length which shows up under "Qty".  Also, you will probably want to create custom content center libraries containing a copy of the existing Inventor structural steel libraries, change the standard so you can find them in Frame Generator and then modify the "Part Number" column to suit your needs. 

[Vadim-the-Engineer]

Sounds like a plan. I will definitely check the option as soon as I get
back to work on Sunday. For now I found some loopholes (custom properties)
to receive the BOM I need but those just patches...

[P_Korgaonkar]

For some Weird reason, it is not working for me.

For the part number, I have a B_L value which works fine, but same B_L value when I add to the description it does not work. Any suggestions to resolve this issue?

Regards

Parag

[cadman777]

I realize this is an old thread, but someone just referenced it in the forum, so I'm adding my 2 cents' worth.

Whenever I had a problem with Family Table iProperties, I just created my own Custom iProperty and used it in the Family Table. For example:

I started using G_L for the length iProperty instead of B_L.

But when I had to change the frame members, the new parts on of the frame would have lengths that lost their units formatting. So I created a Custom iProperty G_LL and used it. I learned that from someone in here a number of years ago, and it works consistently. For some reason, when you remove the original iProperty one step away form the BOM calculation, it maintains its units formatting. I have no idea why.

So if you want to troubleshoot this problem, make a temporary Custom iProperty and replace B_L with it to see if that solves your problem. If so, then I wouldn't waste any more time on trying to figure out the cause of this work-stopping problem. I learned a long time ago that if I can find a work-around for a recurring problem in Inventor, to go with it and DON'T LOOK BACK. Because if it's a DEFECT in the software that Autodesk refuses to fix, I'll probably be dead and buried by the time they fix it! So no point getting hung-up on something I can't change when there's a simple solution to fix the problem.

Incidentally, changing the length iProperty from G_L to G_LL took me about 8 hours of work on my content center and my other customizations. The lesson there is, if you decide to make a work-around, you'de be wise to make sure it fits into your work-flow and other procedures, and doesn't cause other headaches down-line.

[P_Korgaonkar]

Thanks, Chris

Can you post a small video or explanation of how to do this?

I know how to create a custom property on the part level or Assembly level, but not sure how to do this with Content centre parts.

Is the custom property G_LL directly link to B_L or G_L?

Or are you suggesting renaming G_L to G_LL

Thank you once again.

Regards

Parag

[cadman777]

Find attached pdf showing what I do.

Maybe it'll work for you?

I use only the most basic functions of Inventor, so everything I say is based on basic Inventor functionality.

Cheers ...

[P_Korgaonkar]

Thank you, Chris

The attached PDF is Helpful, appreciate your efforts and help.

Will give it a try, I believe it should solve my issue.

Thank you once again 

Regards

Parag

[cadman777]

You're welcome!

Let me know how it works out for you.

[P_Korgaonkar]

Thank you Chris

I gave it a try but could not make it work.

I am using Inventor 2021, and I can not see the options you get on your screenshots.

I can not open the part from CC, I get an option to save the part instead,

Also, I can see the option to update template either.

Regards

Parag

[cadman777]

Sorry for the delay...

You first have to establish a READ/WRITE Custom CC Library.

Otherwise, you can't write to the CC.

You have to write to your Custom CC Library, not the Default Inventor CC Library.

Creating a custom CC Library is easy.

But there's a a bit of a learning curve changing it to suit your needs.

But once you learn it, you can have a lot more control over your work-flow.

Here's instructions on making a READ/WRITE Custom Library:

https://www.youtube.com/watch?v=NkSOMoT2qeQ

Start @ 2:45 and listen till 7:05.

If you already have this, then there's something else that needs to be addressed.

[P_Korgaonkar]

Thanks, Chris

Yes, I have done that and my library is Read/write enabled.

I have attached the Library file and some screenshots.

Please note I am using Inventor ISO SHS library to use for my custom library!

By using this library, I am able to get the description correct as I expect, but the length value is coming in the part number column, I would like to get this value in the Description column. If this can be achieved, then I would like to see the Part number as the file name without extension.

I am unable to get G_L parameter or d18  parameter which is "Length" value in the part parameter. This leaves me only option B_L parameter to use for length value. This brings me to the same question as mentioned above, The B_L value works in part number column, but the same parameter does not work in the Description column. As you may notice, B_L parameter is included in the Part number and Description, but the value is seen only in the part number column of Parts list and to Description column.

As you suggested I was trying to create G_LL parameter to see if that works, but I am unable to create this parameter in the content centre part. I was last trying to use d18 parameter to include in the description column, but I can't do that either.

If you like I am happy to do an online meeting and give you remote access to my pc, we can do this together.

Regards

Parag

[cadman777]

Hi Parag,

OK, here's some things to try:

1. When you use 'Open from CC', you have to save your part. Make it a name that you'll be able to identify as distinct from other similar parts if it's in your current project folder. I usually add a prefix "_Template-".

2. Then modify that part.

3. Then open 'CC Editor' and make your Custom CC Library 'active', but you may need to Update them first (see attached pdf).

4. Then try 'Replace Template', per previous pdf.

5. I think the reason you're getting the wrong number in your Description column is b/c Inventor is reading 'B_L' as the CC part's DEFAULT LENGTH (in the Family Table, RMB on the B_L column > Column Properties, and look at the Expression - Custom Column radio button will be active). I believe the last value between the "[]" brackets is the 'default length' value you're seeing in your Description parameter (same as in your screen shot .001"). That's what Inventor appears to be reading. I think it should not be doing this. Maybe this is a 'bug'/defect in the software? Maybe someone from Autodesk can 'chime-in' and tell you if it is?

I'm having a problem reading your CC library parts even though I migrated them to my older version of Inventor. I can add your libraries to my library (Inventor 2010), but 'Contech Profiles' doesn't show any parts in it, and 'Contech Structural Shapes' causes Inventor to crash when I attempt to open the Family Table. Maybe my version of Inventor is too old to read your library? It shouldn't be, but maybe it is? It's a simple database, so I can't image there's any problem. Maybe Autodesk changed this so it's not backward compatible? Since I can't read your CC library, I'm giving you my 'best guess' at this point, without having looked at your CC library parts.

[cadman777]

Parag,

You can change the Family Table column FILENAME to whatever you want your part file name to be.

See attached pdf screen shot of my CC Family Table for a typical part.

You can construct your file name using a STRING of iProperties, or you can recycle an existing iProperty that has all the info in it already. There's pro's and con's to each method. I have a system so my method works good w/my system.

Cheers ...

[P_Korgaonkar]

Thanks, Chris.

Yes, the library file I sent it Inventor 2021 version, I don't believe any Inventor files are backwards compatible, but I may be wrong.

The library I am using is not one part it is SHS library meaning there are lots of parts in this one library so what you suggest as saving one part as a template file and then change it into the Inventor content centre does not apply/work.

The B_L parameter can work only if it's in the Part Number column of the CC spreadsheet and can only be imported into Part number column of the Parts list in IDW.

I have tried to switch these columns between Description and Partnumber columns but it does not work!.

As you said, yes, there is a bug in the systems and Autodesk is aware of this. Johnsonsui from Autodesk investigated this thread and suggested it may get fixed in future releases. I can't remember which version I was using when I first tried it, maybe 2018.

Thank you for your help, Chris.

Regards

Parag

[cadman777]

Hi Parag,

Thanx for the update.

OK, so let me get this straight:
You are using Inventor 2021 and you can't access "Replace Template" in the CC Editor?

Can you "Open from CC" and Save to local disk?
And can you edit that file the way I show?

Cheers ... Chris

[P_Korgaonkar]

Hello Chris.

Yes, that is correct.

But the reason is different. I am not using a part template. The library I am using is a copy of Inventor library it is using a spreadsheet for various sizes, hence I do not get an option to replace template.

Regards

Parag

[cadman777]

Hi Parag,

I'm not sure what you mean.

But I never use Excel, b/c it has so many problems (as you can see).

Except you can edit the Family Table IN Excel, which is different from haveing Excel as an external data file for a part's parameters. Is that what you're doing with these parts?

Anyway, you may need to Author a new version of your part w/the iProperties I talk about in my 2nd pdf.

That will probably fix the problem for you ... I HOPE!

Cheers ...