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Custom Shapes for Content Center

13 REPLIES 13
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Message 1 of 14
GSE_Dan_A
1837 Views, 13 Replies

Custom Shapes for Content Center

Good morning Inventorees,

 

The time has finally arrived; the current content center profiles no longer suit my needs (for this specific project) and I now must create an extrusion that consists of holes.  This profile is to be used in the Frame Generator and Frame analysis so it is imperative that I get the holes into the custom extrusion (see attached picture for the extrusion I require - it is a column extrusion for Pallet Racks.  I have never entered the realm of custom content center extrusions so I am as they say a "Noob".  Can anyone give me an idea of what I need to do as far as what values I will require for the Analysis part (Inertias, Areas, etc...) and what proces I will take in order to first set up my extrusion to use?  As mentioned, the holes in the extrusion are vital as they occue frequently (every 3 inches) and will affect the results in my analysis. I am currently in the process of reading up on Custom Content Center Publishing, but I figure it is best to ask the Community for their advice.  Using Inventor 2014 Professional.


Any and all help is greatly appreciated.

 

Post.jpg

GSE Consultants Inc.
Windsor, ON. Canada
13 REPLIES 13
Message 2 of 14
GSE_Dan_A
in reply to: GSE_Dan_A

Ok so I have a Custom Content Center Setup, I have my part Published and I can even place it into the Frame Skeleton I have created.  However, the holes, fillets (all features) do not show up when I place the member on my skeleton.  Can anyone advise how to keep the features on my part when I publish to my CC?

 

GSE Consultants Inc.
Windsor, ON. Canada
Message 3 of 14
GSE_Dan_A
in reply to: GSE_Dan_A

Can't seem to get the features (holes, fillets, etc..) to repeat over the length of the member.  For example if the member is 144 inches long, how do I get the holes and extrusions to cover the 144" at 3" c/c spacing? Can anyone attach a part that exhibits this behaviour?

GSE Consultants Inc.
Windsor, ON. Canada
Message 4 of 14
mpatchus
in reply to: GSE_Dan_A

You'll have to do the holes as a pattern.

For the number of holes, create a parameter with a formula that calculates the length divided by the spacing.

Thus, when the length changes, the number occurances will adjust accordingly.

Mike Patchus - Lancaster SC

Inventor 2025 Beta


Alienware m17, Intel(R) Core(TM) i9-10980HK CPU @ 2.40GHz 3.10 GHz, Win 11, 64gb RAM, NVIDIA GeForce RTX 2080 Super

Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below. 🙂
Message 5 of 14
cwhetten
in reply to: GSE_Dan_A

Attached is a piece of unistrut that I modeled & authored for use in frame generator.  I didn't set up any of the parameters needed for frame analysis, but it is an otherwise good example of a part (an iPart, actually) that is set up with a pattern of holes.

 

Cameron Whetten
Inventor 2014

Message 6 of 14
GSE_Dan_A
in reply to: cwhetten

Thank you both for your response.  cwhetten - how is the Driven Length feature created in your part? I notive it exists in CC parts as well. 

GSE Consultants Inc.
Windsor, ON. Canada
Message 7 of 14
cwhetten
in reply to: GSE_Dan_A

The driven length feature should be automatically created by the authoring process.  Here is a simple step-by-step for how to create a basic structural shape:

 

1. Start a new part.

2. Create your profile sketch.

3. Extrude your profile sketch.  Set the extents to "Distance" and give it a value (doesn't matter what this initial extrude distance is, it will be deleted by the authoring process--you just need to have an extrusion to start the authoring).

4. Create a user parameter that will be mapped to the Base Length.  I use PL, since that seems to be the convention for other CC parts.  The initial value of this parameter doesn't matter, but it should be big enough to see any patterns in your part (hole patterns, for instance).

5. Author the part (see image below)

 

CC Structural Shape Authoring.png

 

Don't forget to go to the Parameter Mapping tab and map any of the parameters that show up in yellow (yellow ones are required).

 

The authoring process should create two work planes (Start Plane & End Plane), will rename your extrusion to Body, and will create the Driven Length feature.

 

Once the part has been authored, you can publish it to the content center.

 

Cameron Whetten
Inventor 2014

Message 8 of 14
GSE_Dan_A
in reply to: cwhetten

Many thanks for your help! One last issue I am experiencing is when I got to place my part into an assembly, I can not for the life of me figure out how to manually type in a length.  For example when I place a CC part, I am able to input a specidied member length.  When I attempt to place mine into an assembly, it defaults to my set B_L (3 inches) and I can not edit it unless I go into the part.

GSE Consultants Inc.
Windsor, ON. Canada
Message 9 of 14
cwhetten
in reply to: GSE_Dan_A

Are you publishing this as a content center part, or just placing it like an ordinary part?

 

Also, did you create it as an iPart?

 

Cameron Whetten
Inventor 2014

Message 10 of 14
GSE_Dan_A
in reply to: cwhetten

I published this as both a CC part (to use in future Assemblies) and as a Structural Shape (to use in Frame Generator).  Currently this is not an i-part, but I may change this depending on how often I require this shape (or something similar). For now I just need to wrap my head around Custom shapes and the workflow.  Performing FEAs on parts with many holes causes slow results and often they are misleading due to corners, contacts etc... so the frame analysis will make things much much faster and easier.

GSE Consultants Inc.
Windsor, ON. Canada
Message 11 of 14
cwhetten
in reply to: GSE_Dan_A

I could be wrong on this, but I think the only way to get it so you can specify a custom length when placing is to create an iPart table and set the length parameter (B_L did you say?) as a custom column.  Does that make sense?

 

Even if you only have one configuration of the part (with varying length, of course), you can set up an iPart table with only one row.  Then you would add the length parameter as a column, right-click that column and set it to be custom.  Take a look at the example part I posted earlier.  The PL column in the iPart table is set up as a custom column.

 

I'm not sure this explanation makes much sense, so post back if I wasn't clear enough.

 

Cameron Whetten
Inventor 2014

Message 12 of 14
mpatchus
in reply to: cwhetten

Simply make the LENGTH property a key property in the part family.

This will give you a length dialog box when inserting the part.

Mike Patchus - Lancaster SC

Inventor 2025 Beta


Alienware m17, Intel(R) Core(TM) i9-10980HK CPU @ 2.40GHz 3.10 GHz, Win 11, 64gb RAM, NVIDIA GeForce RTX 2080 Super

Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below. 🙂
Message 13 of 14
AERE
in reply to: GSE_Dan_A

Good Evening GSE_Dan_A, To automatically arrange hole pattern based on part's length, I use iLogic rule (called HOLES in this case) triggered by Part Geometry Change. After the rule is placed, the part is ready to be published. Works perfectly fine with Frame Generator. Please see the attached sample. I used standard W beam part to start with and made distance between holes 3". Change the B_L value and holes will re-arrange...nothing special has to be done in preparation for FEA. Have fun! Serguei Velidtchenko Inventor'2014
Message 14 of 14
AERE
in reply to: GSE_Dan_A

GSE_Dan_A,,

I had problems with loading the file last night but here it is.

 

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