Hello,
I am designing an enclosure, and would like to have a honeycomb cut outs for airflow. Something like the image below from thingverse. What is a good way to do this with F360?
Solved! Go to Solution.
Solved by SallyYang. Go to Solution.
We will mainly use pattern to create this honeycomb, the steps are:
1. Create a sketch like bellow:
2. Extrude the polygon ribbon
3. Rectangular Pattern the body along 2 construction lines in the sketch(Distance type = Spacing)
4. Combine all patterned bodies to 1 body(Operation = Join)
5. Create a box to cut the honeycomb.(Operation = Intersect)
Hope it will help you.
I could also suggest making the hole size you want in your surface, and using the Create- Pattern- Rectangular Pattern. Or you could make an array of objects with the same tool and use a boolean subtraction (Combine- Cut) to get your holes. The pattern tools are very flexible.
I am having trouble with 3rd step. If I try to do rectangular pattern with the extruded ribbon, I get "Failed because could not find intersections to destination". If I do rectangular pattern of sketch, then I do not get the pattern you got. My hexagons are right on top of each other, whereas your rows are offset from each other. What am I missing?
I guess you selected face to pattern when you get the failure. To pattern the hexagons, you can either select the edge of it or select body node from browser tree.
This is something that I think trips up a lot of Fusion users, who come to the program expecting to be able to select bodies in the drawing- to do so requires a specific selection technique (edge selection, if there is an edge), except for some tools that allow only whole body selection. I realize I reflexively now select bodies in the browser tree when I wan to perform any sort of operation on an entire body.
In this case, we could support both face pattern and body pattern, so when you select face, we consider it as face pattern, and when you hover on an edge, , you actually highlight&select the body(as edge is invalid input for pattern) to do body pattern. It's a workaround for selecting body from canvas when both face and body could be valid inputs.
Sorry for the late reply, but I have been away. So yes, selecting body works, but I do not get the same type of pattern as first reply. When I select rectangular pattern, I literly get a rectangular pattern, and not the offsetting pattern you have, whereas the second row is half a column over.
I think you probably select different directions. Please make sure to select the red line as directions.
As the sketch will be auto-hide in modeling envrionment, you have to turn on visibility of sketch file and then select the red lines as pattern directions.
Thanks,
The problem was I didn't realize those construction lines were at 60 degrees, and was doing 90. Much better.
Thanks.
Hi,
@alphaaPDYTU wrote:This requires a lot of processing power to complete this task.
... does not if you use pattern in body mode instead in sketch.
günther
Hi Mr AlphaaPDYTU,
Yes, the hardcore modelling of patterned features will add a bulkiness to the model so it will have an effect on its responsiveness in a design environment. If there are no specific circumstances it should be limited to a specific part destined for manufacturing based on its direct model.
Patterned Appearances of F360 offer lightweight aesthetic simulation of them, being fast and easy at the same time.
Regards
MichaelT
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