What is best way to add honeycomb perforation to panel?

[autodesk]

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?

http://thingiverse-rerender.s3.amazonaws.com/renders/31/15/f8/74/b4/RepExFanGuardH_preview_featured....

[SallyYang · Accepted 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.

[Oceanconcepts]

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. 

[autodesk]

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?

[SallyYang]

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.

[Oceanconcepts]

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. 

[SallyYang]

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.

[autodesk]

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.  

[SallyYang]

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.

[autodesk]

Thanks,

The problem was I didn't realize those construction lines were at 60 degrees, and was doing 90.  Much better.  

Thanks. 

[alphaaPDYTU]

This requires  a lot of processing power to complete this task.  

[g-andresen]

Hi,

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@alphaaPDYTU wrote:

This requires  a lot of processing power to complete this task.  

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... does not if you use pattern in body mode instead in sketch.

günther

[TheCADWhisperer]

File>Export and then Attach your *.f3d file here.

[MichaelT_123]

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