Hello,
I want to arrange hexagonal elements in a circular shape, like this:
The hexagonal element looks like this:
I tried using Pattern (in the combine section), circular, but the elements are placed into each other.
I really don't want to do it manually, because its about 1500 elements.
I hope this is an easy fix!
Thanks in advance!
I am writing an essay about Nuclear Thermal Propulsion.
This type of rocket contains a nuclear reactor with a core arranged out of long, hexagonal fuel elements. (see picture in the fist post).
The element is an assembly. (Fuel element + Coating on the axial surfaces)
The picture above is an excerpt of the fuel element arrangement, the full assembly contains about 1500 of these hexagonal elements.
The elements with the circurlar "interior" are support elements, that I do not need to include.
I hope this answer is sufficient.
Hi! There should be a way to do that with some modeling steps. You don't have to constraint 1500 rods individually. I will share solution later.
Many thanks!
Hi! Here you go! A 10-minute attempt on 2019. It is highly doable using Sketch-Driven Pattern.
Many thanks!
Hi –
I think a “honeycomb” like this is easier to model as a rectangular pattern starting with two hex cells at one corner.
I have attached a 2019 example which uses a sketch pattern of sketch point, and a sketch-based feature pattern based on that sketch. I did need to manually convert sketch points that fall outside of the circle from center points ( + ) to standard points ( . ) so the feature pattern would ignore them. Since you are really doing a one-off this is not too much effort.
The hardest part was positioning the two points at the lower-left corner to start the pattern.
If you will be using an Assembly pattern, you can make the part level Feature pattern a pattern of Work Points, then create the Assembly pattern associative with the Feature pattern. (So, Assembly pattern is based on the Part Feature pattern which is based on the Sketch pattern!).
Hope it helps!
T.0.M.
Elegant solution @johnsonshiue! It's going to take me more than "10 minutes" to figure out how you replicated the center points in the sketch...
Hi @richter2felix,
Nice to meet with someone from Bremen! It is a very pretty town with a lot of history and interesting attractions. Highly recommended! I will revisit someday.
Let me explain how I approached the design. Inventor does not have the ability to do "Filled Pattern" (packing pattern instances within a boundary). Even if it did, "Filled Pattern" would not yield the predictable result like you wanted.
First of all, there is no way you can create the pattern using one patterning operation (circular or rectangular). It is just impossible without having overlapped instances. That leaves the choice to Sketch-Driven Pattern.
Then the focus becomes how to create the points to drive the pattern. Based on the image, there are two groups of points. Group A: the individual points evenly distributed around layers of hexagon boundary. Group B: the 6 outliers.
Next, you need to figure out the spacing between layers in Group A. Essentially, they are on one side of a hexagon (1/6). Add those points and constrain them accordingly. However, you cannot just pattern the points (on one side) together 6 times around the center. You will end up with points on top of points along the diagonals. To avoid that, you further break up Group A into two subgroups: A1) points on diagonals and A2) points not on diagonals. For A1 points, circular pattern 3 instances. For A2 points, circular pattern 6 instances.
Group B is the most straightforward one. You simply circular pattern 6 instances around the center.
Lastly, create a workpoint at the center. And, create a Sketch Driven Pattern (SDP) of the workpoint based on the sketch points. Place this skeletal part in an assembly. Insert a hexagon rod part at the center. Pattern Component based on the SDP.
BTW, the holes in the hexagon rod are populated similarly.
Many thanks!
