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Cannot Create Custom Frame Member Part

16 REPLIES 16
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Message 1 of 17
ARCross
2831 Views, 16 Replies

Cannot Create Custom Frame Member Part

I created a template part, turned it into an I-part and published it successfully as a Frame Member.

 

The custom member was published into a custom library that is read/write.  I was forced to create this library in order to publish the part... I am not sure why.

 

When I go to use the custom profile with the frame generator, I am able to find the custom member in the dialog but when the frame generator tries to generate the part, I get this error message:

 

[WARNING] Frame Generator: Errors occurred during inserting Frame Member(s)
    [WARNING] Insertion of frame member(s) failed
        [ERROR] A frame member could not be created.  The template file for Unnamed GIRT-2 could not be located in the Content Center library.

Any thoughts as to where I am going wrong?  Thanks,

 

Andrew

16 REPLIES 16
Message 2 of 17
Dennis_Jeffrey
in reply to: ARCross

Inventor version please?

Please mark this response as "Accept as Solution" if it answers your question.
____________________________________________________________
Dennis Jeffrey, Author and Manufacturing Trainer, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert
Autodesk Silver Manufacturing Partner

Subscribe to the free digital "The Creative Inventor Magazine" now available at: http://teknigroup....

XP64 SP2, GeForce 9800GT-1GB, Driver: 6.14.12.7061, 8GB Ram, AMD Athlon II 3.2 Ghz
Laptop: Win7-64 Pro, 4GB, ATI Graphics on board, 2012 Ultimate, IV2011 or 2010 Pro, all SP's
Message 3 of 17
ARCross
in reply to: ARCross

Sorry, we are using InventorSeries 2010.

Message 4 of 17
Dennis_Jeffrey
in reply to: ARCross

Did you author it as a structural part?

 

Can you zip and attach the original pre-published part? I'll take a look

Please mark this response as "Accept as Solution" if it answers your question.
____________________________________________________________
Dennis Jeffrey, Author and Manufacturing Trainer, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert
Autodesk Silver Manufacturing Partner

Subscribe to the free digital "The Creative Inventor Magazine" now available at: http://teknigroup....

XP64 SP2, GeForce 9800GT-1GB, Driver: 6.14.12.7061, 8GB Ram, AMD Athlon II 3.2 Ghz
Laptop: Win7-64 Pro, 4GB, ATI Graphics on board, 2012 Ultimate, IV2011 or 2010 Pro, all SP's
Message 5 of 17
whunter
in reply to: Dennis_Jeffrey

Hi all;

 

I get the same error. Inventor 2011, 64-bit. I've attached my 'authoring' file. Any ideas what's going on here? I've done this before and then it worked, must be doing something wrong this time round but I obviously don't know what.

 

Thanks,

William

Message 6 of 17
Dennis_Jeffrey
in reply to: whunter

Question: What is this? See attached.

Please mark this response as "Accept as Solution" if it answers your question.
____________________________________________________________
Dennis Jeffrey, Author and Manufacturing Trainer, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert
Autodesk Silver Manufacturing Partner

Subscribe to the free digital "The Creative Inventor Magazine" now available at: http://teknigroup....

XP64 SP2, GeForce 9800GT-1GB, Driver: 6.14.12.7061, 8GB Ram, AMD Athlon II 3.2 Ghz
Laptop: Win7-64 Pro, 4GB, ATI Graphics on board, 2012 Ultimate, IV2011 or 2010 Pro, all SP's
Message 7 of 17

Is this a custom notch shape?

Please mark this response as "Accept as Solution" if it answers your question.
____________________________________________________________
Dennis Jeffrey, Author and Manufacturing Trainer, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert
Autodesk Silver Manufacturing Partner

Subscribe to the free digital "The Creative Inventor Magazine" now available at: http://teknigroup....

XP64 SP2, GeForce 9800GT-1GB, Driver: 6.14.12.7061, 8GB Ram, AMD Athlon II 3.2 Ghz
Laptop: Win7-64 Pro, 4GB, ATI Graphics on board, 2012 Ultimate, IV2011 or 2010 Pro, all SP's
Message 8 of 17
whunter
in reply to: Dennis_Jeffrey

 


@Dennis_Jeffrey wrote:

Is this a custom notch shape?


 

Yes.

 

Background: I'm evaluating if we can use Inventor for our designs (currently using Bentley ProSteel with AutoCAD), the only thing stopping us is the ability to model structural end connections with coping/bolting/plating. I thought of using Revit, but we also do a lot of mechanical work, more than structural, on the same projects (typical of modular mining plants), so...

 

The only option I see is a combination of custom notches and iFeatures and/or iCopies. There's the API too, of course, but that's a lot of work/time.

--

wh

Message 9 of 17
Dennis_Jeffrey
in reply to: whunter

This part ( made from your sketch) works. Check the table differences.

 

Note that I did nothing with file naming or descriptions.  Fix your part first, then work on those. Resources on Content Center descriptions, etc. are available in the March/April issue of The Creative Inventor Magazine.

 

You might want to review this document:

 

http://teknigroup.com/AU2008

 

I'll be back at AU this year with an enhanced version of this subject.

Please mark this response as "Accept as Solution" if it answers your question.
____________________________________________________________
Dennis Jeffrey, Author and Manufacturing Trainer, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert
Autodesk Silver Manufacturing Partner

Subscribe to the free digital "The Creative Inventor Magazine" now available at: http://teknigroup....

XP64 SP2, GeForce 9800GT-1GB, Driver: 6.14.12.7061, 8GB Ram, AMD Athlon II 3.2 Ghz
Laptop: Win7-64 Pro, 4GB, ATI Graphics on board, 2012 Ultimate, IV2011 or 2010 Pro, all SP's
Message 10 of 17
ARCross
in reply to: ARCross

Sorry for the delay in getting back to you.  I think part of our problem was a faulty installation of Excel. 

 

I also redid the part -  a custom girt.  Here was my workflow:

 

1.Create profile sketch:

2. Extrude sketch - use a parameter labelled 'length'

3. Turn part into an i-part - create table that allows for multiple widths of girt.

4. publish as a structural member - in the parameter mapping dialog - enter 'LENGTH' for the 'BASE LENGTH' box.

5. Publish

 

I had to create a read/write library under the edit projects dialog box - far bottom right corner, click libraries button and create new library.

 

Anyway, it seems to be work now although I need to do some more work in order to get the part showing with necesary information in the BOM.

 

AC

 

PS - I have been working on the part on a new computer that doesn't have interenet set up. Otherwise I would post the post the part for critique.

 

Message 11 of 17
ARCross
in reply to: whunter

I would be interested in finding out how that works out for you.  Most of our work is also mechanical but we do the odd structure.  Anything that can be inserted using the frame generator is great but I have puzzled over what is the right workflow for inserting gussets and end connections.

Message 12 of 17
whunter
in reply to: ARCross

AC;

 

I fiddled with a custom notch and end plate yesterday, it seems to work, but the help file warns that one shouldn't add fearures to the base profile as it might give unexpected results...

 

I'm starting a new thread: Bolted Frames and End Connections. I'll post what I've accomplished (or NOT) there.

--

wh

Message 13 of 17
whunter
in reply to: Dennis_Jeffrey

Thanks, Dennis.

Message 14 of 17
csmac2004
in reply to: ARCross

Just to bring up ghosts from the past... 🙂

 

I found this discussion today while trying to figure out why my custom created content centre files kept giving me the same error message as per the OP's first post here. No matter what I did, it just will not work.

 

I am running Inventor 2011 with Microsoft Office 2010, which I think is my problem. The final post by the OP stated that he had to repair his Office installation. Well, as I look into this, I have noticed that there is no support for Office 2010 yet, so I am guessing that is the case here.

 

So, I'm just posting this for anyone else that may be hitting their heads against a wall on this one as well. Not sure what I'm going to do to get around this, but that is what I have discovered in my travels today... 😞

Scott MacDonald
Inventor 2013 Product Design Suite
Vault Professional 2013
Windows7 x64
Autodesk Inventor Certified Professional
Message 15 of 17
tsreagan
in reply to: ARCross

Once you create a frame member part,  where is the template file located? I deleted the original and there are no errors, so I assume the Content center saves a template somewhere, and its not in the documents/inventor/contentcenterfiles folder.

 

One problem is that some parts have missing vendor info,  which I forced in the family table by adding a column and mapping it.

 

The other problem I cannot fix,  the BOM structure needs edited, and I see no way to access these parameters from the family properties or table.

 

 

Inventor 2013

 

Thanks

 

ARC

 

Message 16 of 17
tsreagan
in reply to: tsreagan

I rebuilt the members from scratch to fix the BOM structure issues.

 

If someone could still clue me in as to the location of templates, or some way to access these paramaters after members have been created, it would be greatly appreciated.

 

FYI

If others are having issues with a particular frame member not getting the right part number assigned,

make sure your lengths for structural shapes are set to .001 like the stock library items.

 

I always wondered why they used .001 to start. 

It appears if a generated frame member length = the length of the default content center member then it will not properly generate part numbers for the member.

 

I was using 12in as my generic start length in the content center. It was just chance that my skeleton wire frame for testing content center parts had a few 12in wires, and when the members were generated over top of them, the part numbers were always wrong untill i changed the default length to .001.

 

 

ARC

 

 

Message 17 of 17
Edward_Lowe
in reply to: ARCross

I know I am very late to this party but thought I should share my experience with you.

 

I struggled for days to work out why this error message appeared.  Eventually our Inventor Support Company worked out the ilogic I introduced with the part file interferred with the publishing process.  When using the standard part file (without ilogic) the publishing process worked without a problem.

 

Hopefully this will save many hours of head scratching.  Thanks again to our support company, Quadra Solutions Ltd,

 

Regards,

 

Edward

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