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
Did you author it as a structural part?
Can you zip and attach the original pre-published part? I'll take a look
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
@Anonymous 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
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:
I'll be back at AU this year with an enhanced version of this subject.
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.
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.
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
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... 😞
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
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
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
Can't find what you're looking for? Ask the community or share your knowledge.