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Posts: 23
Registered: ‎07-24-2012
Message 31 of 38 (308 Views)

Re: Feature driven Pattern

09-13-2013 09:36 AM in reply to: seytayfun

however after retrying we were not able to achieve our goal as Inventor wasnt able to recognize INSERTION POINTS. We are able to make holes in part with insertion points. but when we tried to pattern the rod in assembly it just does not recognize the insertion points or holes feature. Or we miss something. Is it possible to insert (distribute) a part by predefined points (exp. from excel) or sketch?

Attached is the example that we want to achived. Please try to pattern (distribute) the rod into holes by one command

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Posts: 1,170
Registered: ‎06-19-2006
Message 32 of 38 (306 Views)

Re: Feature driven Pattern

09-13-2013 09:51 AM in reply to: seytayfun

In order for an assembly pattern to recognise an array of features, you must make that array with the feature pattern tool in the part file.  When you do that, constrain the object that you want to pattern in the assembly to the base feature of your pattern.  JDMather's idea of changing the color of the base feature is very helpful. 


If you are trying to make a single sketch with an array of centerpoints, the assembly pattern tool will not "see" that array.  Even if you use a sketch pattern to create the array of centerpoints, the assembly pattern tool will not "see" that array.  You will have to constrain each component individually.  This is the main reason that I avoid placing more than one centerpoint in a sketch that locates a hole.


If you create an ipart factory with a pattern feature and you place a member in an assembly, the assembly pattern tool will not "see" that array in any of the members.  The derive operation that creates members from the factory hides the pattern feature.


Do note that you can pattern patterns in parts and assemblies.

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Posts: 26,181
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Message 33 of 38 (295 Views)

Re: Feature driven Pattern

09-13-2013 10:36 AM in reply to: seytayfun

Can you attach a real assembly - I would not consider this good modeling practice in Inventor or SolidWorks.

You should be able to make something up that exhibits all the behavior of your proprietary work without giving anything away.  (I could do it myself from looking at your previous screen capture, but -.....)

Please mark this response as "Accept as Solution" if it answers your question.
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Posts: 23
Registered: ‎07-24-2012
Message 34 of 38 (283 Views)

Re: Feature driven Pattern

09-13-2013 11:24 AM in reply to: JDMather
JD. it s simple. just distribute the rods inside each holes by pattern. Do it anyway you like. it's so clear what I need. You know that is very easy in Solidworks. i am getting feeling that is just NOT possible in Inventor. We work with heat exchangers that requires lots of tubes (which i call rods here) inside a container. Thus, we do not want to insert each tube one by one which will take lots of time and effort to control.
Posts: 23
Registered: ‎07-24-2012
Message 35 of 38 (277 Views)

Re: Feature driven Pattern

09-13-2013 11:31 AM in reply to: seytayfun

Since I am about to cross out feature pattern option by center point, Would anyone recommend me to achieve this by a trick through " Bolted Connection Component Generator"? Perhaps somehow insert (or save) my tube (rod) as a Fasterner inside BCCG and then distribute (pattern) it as fastener? 

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Posts: 2
Registered: ‎09-15-2013
Message 36 of 38 (235 Views)

Re: Feature driven Pattern

09-15-2013 09:30 PM in reply to: seytayfun



I have come from an SW environment & always used sketch based pattern but as we all know, Inventor lacks such a feature.  I came up with a work around which gives you point locations at varying spacing aligned or any point required.


See this thread I posted earlier:


This works if points are not alligned also - just ensure the zig-zag curve does not cross over itself.

See attached Image.


Hope this helps - it has certainly helped in my application.

Posts: 23
Registered: ‎07-24-2012
Message 37 of 38 (202 Views)

Re: Feature driven Pattern

09-17-2013 11:28 AM in reply to: forbillian

Thank you very much forbillian. I have tried your method and yes it works. However drawing equal curve lines between at least 50 points is a challenge and sometimes impossible as some locations are too close to each other. So we are locating tubes by small patterns or individually for now.

Posts: 5
Registered: ‎09-27-2013
Message 38 of 38 (184 Views)

Re: Feature driven Pattern

09-27-2013 07:38 AM in reply to: CAD-One

I am an imigrant from SolidWorks. In SW you can insert a part or assembly on a hole, then using the "Feature Driven Pattern" command, you can have that component repeat on all of the same holes made in a single hole feature operation, just by picking any of those holes. These holes were made with a traditional sketch that is dimensioned according to your needs. For example if you have a plate that has 4 mounting holes, all are 1/2" from the edges because that's the way the sketch is done. This means that if you change the size of the plate, the holes change with it and are always 1/2 from the edge. It appears that the only way to use Inventor's "Pattern" for the inserted component is to pick a "patterned" set of holes. Well, this makes absolutely no sense from a design standpoint, because placing one hole then patterning it, totally loses the parametric aspect of editing. If I change the size of the plate, the pattern does not automatically change. This means I would have to go an extra step and change the holes' pattern. (senseless).

Am I missing something. I discovered that a Content Center item when placed can be chosen to do all holes at the time of the placement only.( I'm gonna take this opportunity to say that I have found it takes about 3 times as many mouse clicks to do same thing in SW)

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