Honeycomb Array
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Honeycomb Array
Hi,
I am trying to model a honeycomb shaped solid whereby I can change the wall thickness and the dimension of the openings later on. So I used the Part Design WB to make a single walled hexagon with parametric dimensions.
Next I tried making a polar array of six of them, but failed because I could not offset the array members to be lined up with the outside walls of my original hexagon.
Then I made a mirrored object with the mirror surface being one of the outside walls. That works, and I did this six times to arrive at this: But now I am stuck, I cannot mirror the original hex wall object with one of the outside walls of the larger honeycomb outside walls any more.
As far as I got, everything is linked with the original and changing the dimensions in the one sketch adjusts everything correctly, but now I am out of ideas.
Cheers,
Chris
OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
Branch: releases/FreeCAD-0-15
Hash: 244b3aef360841646cbfe80a1b225c8b39c8380c
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
I am trying to model a honeycomb shaped solid whereby I can change the wall thickness and the dimension of the openings later on. So I used the Part Design WB to make a single walled hexagon with parametric dimensions.
Next I tried making a polar array of six of them, but failed because I could not offset the array members to be lined up with the outside walls of my original hexagon.
Then I made a mirrored object with the mirror surface being one of the outside walls. That works, and I did this six times to arrive at this: But now I am stuck, I cannot mirror the original hex wall object with one of the outside walls of the larger honeycomb outside walls any more.
As far as I got, everything is linked with the original and changing the dimensions in the one sketch adjusts everything correctly, but now I am out of ideas.
Cheers,
Chris
OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
Branch: releases/FreeCAD-0-15
Hash: 244b3aef360841646cbfe80a1b225c8b39c8380c
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
- wandererfan
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- DeepSOIC
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Re: Honeycomb Array
For a moment, I thought I came up with a method... but it doesn't work. Anyway, it looks cool
- Attachments
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- hex_tiling_experiment.FCStd
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- DeepSOIC
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Re: Honeycomb Array
And sure enough, there is a much simpler method that works
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- hex_tiling_skewed.FCStd
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Re: Honeycomb Array
Interesting use of Draft PathArray tool.
Re: Honeycomb Array
I had some spare time therefore this is the result:
After changing Hexagon size and/or Wall Thickness user has to manually re-calculate and set properties for Draft Array:
Interval X
x = "hexagon radius" * 3
Interval Y
y = ("hexagon radius" * 2) / 1,1547
This limitation should hopefully be easy to overcome once Spreadsheet PropertyController is re-introduced in FreeCAD!
- Sketcher: Create Sketch with Hexagons
- PartDesign: Pad
- Part: Mirror (YZ Plane) and create Pad Mirror
- Change Sketch Angle Property: 30°
- Change Pad Mirror Angle Property: 60°
- Part: Make Compound (Pad + Pad Mirror)
- Draft: Draft Array on Compound
- Sketch (Property View) controls Hexagon Size and Wall Thickness.
- Draft Array properties Number X and Number Y controls number of copies in each direction.
After changing Hexagon size and/or Wall Thickness user has to manually re-calculate and set properties for Draft Array:
Interval X
x = "hexagon radius" * 3
Interval Y
y = ("hexagon radius" * 2) / 1,1547
This limitation should hopefully be easy to overcome once Spreadsheet PropertyController is re-introduced in FreeCAD!
Re: Honeycomb Array
That could help as well since we have OpenSCAD workbench: http://blog.firszt.eu/index.php?post/20 ... rst-battle
TD;DR; Open OpenSCAD wb, click Add OpenSCAD element and paste this: http://firszt.eu/openscad/honeycomb.scad
TD;DR; Open OpenSCAD wb, click Add OpenSCAD element and paste this: http://firszt.eu/openscad/honeycomb.scad
Re: Honeycomb Array
Indeed and i made and attached OpenSCAD example:
I had some fun with OpenSCAD and followed this interesting tutorial:
I had some fun with OpenSCAD and followed this interesting tutorial:
Re: Honeycomb Array
All these arrays need to be trim(m)able, like ulrich1a 's on page viewtopic.php?f=3&t=9963&p=80657&hilit= ... tal#p80657. With ulrich's, you can bool to trim.
My HoneyComb matrix looks good but blows up during bool operation.
Anyone have a version that is trimable?
I need it for actual bees.
My HoneyComb matrix looks good but blows up during bool operation.
Anyone have a version that is trimable?
I need it for actual bees.
Re: Honeycomb Array
If I am understanding what you mean by trimmable, then maybe something like this -bill wrote:All these arrays need to be trim(m)able, like ulrich1a 's on page viewtopic.php?f=3&t=9963&p=80657&hilit= ... tal#p80657. With ulrich's, you can bool to trim.
My HoneyComb matrix looks good but blows up during bool operation.
Anyone have a version that is trimable?
I need it for actual bees.
Check the Array for self intersects before attempting any Boolean operations with it. Depending on how you made the array, you may need to make Array Fuse = true like I did with my model to get it to work correctly.
Mark
OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.5006 (Git)
Build type: Release
Branch: master
Hash: 1099b23587259c7d939a1b5593e6e534b421565a
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
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