I am attempting to add some of our custom extrusions to the content center but want them to act the same way Inventor's "default" files act. By that I mean, if I make a new assembly and pick a piece of Angle, for example, to place from the content center, as long as I choose "as standard" and give it a length, the part shows up without me having to save anything new. I can then copy or drag in a second instance of that same angle, right click it and "change length", and the length of just that ONE changes. In the tree on the right the result is:
DIN 59 370 S S 10x 2 - 600:1
DIN 59 370 S S 10x 2 - 2000:1
With 600 and 2000 being lengths. That's standard Inventor behavior with their standard parts. When I try to publish my own extrusion, I guess I don't have the right key columns or something. I place MY extrusion and input a length, etc. Then when I copy it and try to "change length", nothing happens and it is named part number:2 in the tree.
What am I missing?
Solved! Go to Solution.
As a part but I apparently don't know the correct way to do this. It doesn't matter what my part is, even something simple like a long square 2x2 tube. I want it to behave EXACTLY like the extrusions and structural shapes that came packaged with Inventor. I'm unsure how they have those parts published to allow each length to be changed individually while keeping the same part number. You can see what I mean by starting a new assembly, place from content center, pick any structural shape (like C-Channel or Angle), place it in as standard, copy that part and paste it in the same assembly, then right-click the second part, go to "change length" and enter a new length. The two maintain the same part number but have different lengths.
Well, I followed your workflow and I think I see what you are talking about, but I am not sure what you mean when you say that the two parts have the same part number. They aren't the same:
But, if I understand you correctly, then my first guess is that the issue you are seeing is a result of how you set up the file naming for the published part. Below is what I see when I look at the file naming of the standard Inventor part:
Notice that the file name is built from a combination of text and parameters. One of the parameters is the length of the part. So, when you place a part that is 6 inches long, 6 is a part of the name of the file that is created. When you right-click and "Change Size" to a different length (12 inches, say), it actually replaces the copy with a new part, and this part has a file name with 12 in it.
I am guessing that your published part doesn't take this into account, and maybe it ends up replacing the copy with the same file name as the original (basically, it replaces it with itself, resulting in no change).
Hopefully this explanation made some kind of sense.
Aha, it does make sense. I will try that. I didn't explain the "same part number" correctly at first but you got what I was saying. I will play with that and see what I can come up with.
Do these parts need to be published as iParts with the "Length" as a key column?
On the "publish Part" dialogue, what exactly is the "Map Family Columns to Category Parameters" screen all about? Mine is always blank but the standard Inventor parts have all that filled out... I didn't find much explanation in the help
Yes, these parts should be published as iParts with the "Length" column as a key column.
The content center has several categories of parts. Fasteners, structural shapes, tube & pipe, etc. Each category has certain important parameters that are critical to the way Inventor uses and creates these components. Which parameters are critical is different for each category. Many of the parameters in the list are optional, but, depending on the category, a few are required for Inventor to fully utilize the part.
The "Map Family Columns to Category Parameters" step of the publishing process is mostly for review, because if the part was created properly, it should already be filled out when you get to publishing. This parameter mapping is taken care of in the "authoring" process. The authoring command is found on the Manage tab > Author panel > Structural Shape (it's found under a drop-down that may default to Component or Tube & Pipe).
The parameters that are required to be mapped are highlighted in yellow. In the file I am looking at now (in the Tees category), there is only one required parameter--Base Length. (I suspect that Base Length is the only required parameter for any of the categories under Structural Shape, but don't quote me on this.)
So, you would use this parameter mapping tab in the authoring command to tell Inventor which parameter in your model represents the base length of the feature. The standard content maps to a user parameter called B_L. If you already have a user parameter controlling the length of the extrusion, map the Base Length to this parameter. If you don't have a user parameter for this, I recommend you make one for this purpose.
The other parameters are not required, but some are used by the design accelerators, such as the beam calculator. If you want your extrusions to be able to function this way, you might consider mapping those parameters as well. Take a look at some of the standard content to see which ones might be helpful (see the image below for the specific Tee shape I was looking at).
Edit-- I attached an iPart file (version 2012? maybe 2011?) of a structural shape that I created a couple of years ago. For your reference. I created a custom category for this called Unistrut and published it there.
That was the ticket sir, adding the length parameter to the file name.
Also, how does one delete, move, etc. published parts in the Content Center?
I have several extrusions that were published as regular parts in the Content Center. Is there any way of turning them into iParts while in the Content Center or do I have to edit the original part and re-publish it?
EDIT: I'll take a look at your unistrut and see what I can figure out. Thanks again,
Edit again: I figured out how to delete but not move folders within the Content Center editor.
Also how does one make it default to "as standard" when placing something from content center?
You can delete part families through the Content Center Editor, found on the Manage tab (unless you have no documents open, then it's on the Tools tab). If you want to delete families, make sure your library view is set to your custom library (not merged, see image), otherwise there won't be an option to delete.
If you have the original file you used to publish, I would recommend just deleting the broken families from your CC and republishing them. I also recommend keeping your original iParts, in case you ever have to republish in the future.
As far as moving families in the CC, I don't think you can move them to different categories once they have been published. I could be wrong about this, but I don't know of a way to do it. If you want them to be in different categories, you will have to delete and republish them into their new categories.
Please click "Accept as Solution" if this response answers your question.
Glad I could help! Thank you for marking the solution, it's very helpful for others who might search for this topic later.
...how to make my new content center parts come in by default "As Standard" instead of "As Custom"
This is controlled by your application options. Tools tab > Application Options > Content Center tab > Custom Family Default
If Inventor sees that a CC family has a custom column, it will follow the above setting.
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