Hello,
Can we do a Feature driven pattern in Inventor?
I dont have any parts to share, but can explain my requirement.
I have a assembly file consisting of couple of parts. One of the part is rectangular plate with a several square holes. These In the part level these Sq holes are created using a rectangular pattern.
At the assemb;y level, I want to insert a square plug (plastic Cover) that closes these square holes. I need to know if we can link this pattern to the Original rectangular pattern at the part level.
I have used this kind of feature in solidoworks & its called as Feature Driven Pattern. I need to know if this is possible here.
If so, It makes it so easy to install these covers to all the holes. & when the original hole pattern changes, the cover pattern automatically updates at the assembly level.
Thanks
Solved! Go to Solution.
yes, it works just like SW.
Ribbon: Assemble tab Component panel Pattern
Associative tab
Selects the feature pattern with which to associate the assembly pattern. Displays feature pattern name in the Feature Pattern Select box. Components are patterned relative to the placement and spacing of the feature pattern. Changes made to the feature pattern automatically update the number and spacing of the components in the assembly pattern. Constraints associated with the patterned component are replicated and honored in the assembly pattern. |
You might want to read this document - there is an example of a curve driven Feature Pattern and a subsiquent component pattern in the assembly.
http://home.pct.edu/~jmather/skillsusa%20university.pdf
Tip 46 pg 17
I found this old thread which partly answers to my question:Can I based the "Feature pattern select" on a Hole feature, and not just some array/pattern in the part?
Lets say i'm in an assembly, and want to pattern the parts I have (let's say nuts) according to the hole feature of some part, which will position the parts exactly as i need and in the correct QTy.
I tried to choose the hole feature but it's not letting me choose that...
How do I do that?
Attach your files here.
Hi,
It will be a problem for me to do it now, I dont think I'm alowed to upload here.
but my question is: Is there a way to pattern components based on a hole feature in a part? - exactly the way you can do it in Solidworks, and not just according to an existing pattern in a part...
Thanks!
See if this helps
@Anonymous wrote:I found this old thread which partly answers to my question:Can I based the "Feature pattern select" on a Hole feature, and not just some array/pattern in the part?
Lets say i'm in an assembly, and want to pattern the parts I have (let's say nuts) according to the hole feature of some part, which will position the parts exactly as i need and in the correct QTy.
I tried to choose the hole feature but it's not letting me choose that...
How do I do that?
If I'm understanding you correctly, you don't. It sounds like you have a single hole feature that creates multiple holes. That will not work for the Feature Pattern select, because it is not a pattern. However, if you can instead create your holes by making the first one, and then patterning that hole to create the rest, then it will work.
You may also want to look into the Bolted Connection Generator, which I believe would work with your existing situation.
Using the Bolted Connection Generator you can select existing holes (see attached) or existing patterns.
Hi,
This is very usefull, but can I use to place my own parts, and not just bolts?
If I could do it with my own parts, then It's the most similar thing to "sketch" or "feature" driven pattern you have in soldworks and I would expect Inventor to have something like that by 2012:-)
@Anonymous wrote:...similar thing to "sketch" or "feature" driven pattern you have in soldworks and I would expect Inventor to have something like that by 2012:-)
Been able to do sketch (with a trick) or feature driven (no tricks) part placement for as long as I can remember.
Attach your files here.
Can you try to explain if you possible?
I have a problem with uploading the files in here...
I'd really appreciate your assitance, so will be able to use this "trick" of yours:-)
Thanks!
See pgs 16-18 http://home.pct.edu/~jmather/skillsusa%20university.pdf
in Inventor (or SolidWorks) it is almost always better to use a Feature Pattern rather than a Sketch Pattern.
A feature pattern is needed, but geometry is not needed (my example uses geometry).
To use only a sketch you do need one Feature, but not solid geometry.
That feature is a Workpoint which you then pattern like it was a sketch point.
I just realized that I left out information in TIP 41 (this was intended for a live demo).
See Tips 55-57 here http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf
Hi JD,
As I wrote initally - I didn't mean just "sketch drive" - I also wrote "feature driven".What I meant is to pattern components according to a hole feature, or its sktech. (Holes position)
I'll check what you just sent, hopefully this is the way:)
Hi JD.
I now see that you didn't understand me: I'm not looking into doing a pattern in a part - I want to pattern components in an assembly, based on a hole feature.
Is it possible in Inventor?as I said, in Solidworks it can done according to a "feature driven" or "sketch driven" options.
Thanks!
i hae looked many places and tried many methods. this simply is not possible in inventor! what a shame!! lets og back to solidworks!
@seytayfun wrote:
i hae looked many places and tried many methods. this simply is not possible in inventor! what a shame!! lets og back to solidworks!
Yes, it is possible. I think both of you missed the instructions.
Attach your files here and I'll show you how.
http://www.youtube.com/watch?v=6PJveM-snyE
This is what we need to do. In solidworks you can do that with anything (not only hardware parts like screw, nuts etc..) Think of a rod or spring or a even an assembly of a pen instead of screw in this video and tell me if it is possible to distrubite copies of that part or assembly on the predefines points (like in a curve or sketch) or centers of a feature (like hole or any extrude) same like in this video.
Also in this video after 4:20
http://www.youtube.com/watch?v=uxCEmgDVMMs
Thanks