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
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.
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 -.....)
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?
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.
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.
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)
you wrote:"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. "
This addresses exactly what I tried to achieve because I still think „SolidWorks configurations“. Please find the attached picture.
Is there a workaround to utilise associative component patterns within an assembly containing ipart members?
The derive operation that Inventor uses to create the ipart member from the ipart factory destroys the feature pattern information that the assembly component pattern tool needs.
I think there is a workaround that you can use. You will need to export the dimension parameters that drive the feature pattern in the ipart to the assembly. Once those dimensions are available in the assembly, create a pattern and use them to drive the count and offset dimensions of the components.
for some information about how to link parameters between models. I don't have an example that I can post, so you will have to experiment to get it to work.
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