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,
Inventor version please?
Did you author it as a structural part?
Can you zip and attach the original pre-published part? I'll take a look
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.
Question: What is this? See attached.
Is this a custom notch shape?
Is this a custom notch shape?
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.
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.
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.
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.