Adding personal profiles to the library

[kamenov71]

Hello, I don't remember writing in the forum, but for a few days I've been nervous because of a problem with my profiles that I added to the library. It's about the notorious problem with varies in the details list. Can someone explain exactly how to formulate the profiles when adding to the library so that there is no problem with varies, also how to set up the Family table of the profile group. I read everything I found, but I didn't find a working solution. If possible, the explanation should be with screenshots because of the language barrier. I would be very grateful for the help. I've been working with Inventor for 10-12 years and I'm constantly amazed at how difficult it is when the user has to customize something. Unfortunately, with the competitor Solidworks, these things are child's play, for example, I can give exactly the addition of personal profiles as well as others. Maybe Autodesk will think about this, I hope. I used to participate in the feedback program, but currently I don't have the opportunity to do so. Thanks again.

[jnowel]

If you may, can you add screenshots of your issues so we can understand better?
Assuming you refer as "custom content center" as "personal profiles", how did you set them up?
Did you have a column that would provide "unique" part numbers per size?

Is this post relevant to your issue?
Solved: Re: Base Quantity of Custom Frame Generator Profile Shows as "Varies" - Inventor - Autodesk ...

[kamenov71]

 

 

 

 

 

 

 

 

[kamenov71]

I don't know if you will find your way around. There are also inscriptions in Cyrillic.

[jnowel]

did you perhaps overridden their part numbers?
these 2 items share the same Partnumber but they differ in the lengths

Have you tried doing a "Refresh"?

[jnowel]

I managed to somehow replicate the behaviour using standard content center libraries.
This might be a bug or limitation of the Frame Generator being the difference is quite small (in microns)

Unfortunately, I don't have a solution for this.
maybe @johnsonshiue can investigate and explain further.

To replicate the behavior, I just created 2 sketch lines with 2 different length and inserted the frame members.
you can even increase/decrease the lengths by a minimal value (~20 microns), and the resulting frame member length won't change

[Roman_Vesely]

Hi Krasimir,

 here is the link to topic : How to publish custom profiles in Inventor to be used with the Frame Generator 
Please give it a try and let me know if it was helpful for you.

Best Regards

 Roman

[kamenov71]

Thanks for the help, both of you, I'll check out Roman's link and share the results!

[jnowel]

@Roman_Vesely 
I believe the current issue discussed is due to some bug/limitations in FrameGenerator.
If a steel section is inserted via FrameGenerator, the length in the PartNumber field is rounded up to 2 decimal places (in metric) but the "Base QTY" is computed in 3 decimals.

So, there may be cases (like above) where 2 frame members share the same (autogenerated) PartNumber but having different "Base QTY".

But if a steel section is inserted via "place from content center", the PartNumber field can accommodate more than 2 decimal places. 

I'm not sure if there is a setting that can change the precision of the Length portion in the (autogenerated) PartNumber for FrameGenerator components.

The easiest workaround is to just override the PartNumbers so they don't Merge in the Partslist or BOM Row (as resulting sections with miniscule length differences are quite uncommon)

I just don't want @kamenov71 to chase some "ghost" in their custom profiles trying to figure things out if the issue can be replicated by the standard/built-in sections.
Btw, I'm using Inventor 2026.2

[kamenov71]

 

 The first is with a custom profile, the second is with profiles from the content center. In my opinion, the problem is in the creation of a custom profile family. Inventor does not take into account the unit length of the details if they are created from a custom profile. I know that I can turn off grouping, but then details of the same size are not summed up in the part list. I have some memory that I have worked with a custom profile before and I have not had problems, but it was a long time ago and otherwise I am with 2026.02.

[jnowel]

Yeah. there's is something wrong with your setup with the 20x20x2.

But your settings in 30x30x2 (as seen in the screenshots in message#3) seemed fine.
I wonder why you created a new family instead of adding a new row in the 30x30x2 Family and just rename the family to be generic "SHS - Aluminium" or something

(complete the necessary cell values as needed)

anyway, I still hope to get some insights from them about the issues described in message#9.
I know the few micron differences is negligible in actual fabrication for frames. but can be annoying when one encounter that "varies" unexpectedly.

[kamenov71]

I was just experimenting with different profile families, I tried both I-part and stand-alone profiles, but the result is the same. In message 3, the list is more or less fine because I had changed the base length of the expression by entering values. Pay attention to screenshot 5. I saw this again somewhere in the forum, the advice was from Johnson Shiue. In my opinion, we should not enter values ​​manually, and after a profile is published in the content center in the part list, everything should be fine.

[kamenov71 · Accepted solution]

Hello, I think I found a solution to my problem and I will share it if anyone needs it anyway. Maybe it is not the best solution but it works well. You need to have your own library with read and write. Select from the content center a family of profiles similar in characteristics to what you want to do and copy it to your library with the save as option. Open any profile from the copied family, change the user parameters as you need and save it. When saving, Inventor will not agree but still save it. Open the profile sketch and change it as you need, I drew it again, and assign it the parameters from the "fx" table and save the profile. Open the content center and right-click on the copied family, select replace family template and specify the revised profile that you saved. That's it, then you can change the column names or whatever you want from the family table. In conclusion, I want to say that Autodesk needs to think about making things easier for users. All the changes we need to make are extremely complicated for the average user, I might repeat myself, but with competitors these things are elementary. I like Inventor, but using it can sometimes be a big challenge.

[Roman_Vesely]

Hi Krasimir,
thank you for your feedback.
 
What you described above is how it works now by design. If you want to propose a change in the workflow how to Publish or modify custom families, put your thougths into the Inventor Idea Station : https://forums.autodesk.com/t5/inventor-ideas/idb-p/inventor-ideas-en, please.

Regards

 Roman