Octahedron design

[cubegoldberg]

Hello, I'm quite new to FreeCAD (literally just downloaded) and have had some previous experience with other drafting software. For an initial exercise, I was going to attempt constructing an octahedron. I began with the initial triangle, but am not able to figure out how to construct an additional plane at an angle of 109.5 degrees.

System info:
OS: Windows
Word size: 32-bit
Version: 0.14.3700 (Git)
Branch: releases/FreeCAD-0-14
Hash: 32f5aae0a64333ec8d5d160dbc46e690510c8fe1
Python version: 2.6.2
Qt version: 4.5.2
Coin version: 3.1.0
SoQt version: 1.4.1
OCC version: 6.5.1

[quick61]

Try this, use a cube in wireframe display mode for construction, build the faces for half, from either Draft Line or Draft Dwire, then in Part Worrkbench Fuse, Mirror, Fuse, then convert to solid. Easy...

Octahedron.png (19.89 KiB) Viewed 3416 times

Octahedron.fcstd

(28.97 KiB) Downloaded 105 times

Mark

OS: Ubuntu 14.04 LTS
Word size: 64-bit
Version: 0.15.3765 (Git)
Branch: master
Hash: b5b929cf5822dad2b6622ab7593a112dd2c6b8f4
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
SoQt version: 1.6.0a
OCC version: 6.7.1

[wmayer]

Here is one way how to create an octahedron.

First step:
Go to Part design and create a sketch and add a rectangle there. Make sure that the origin is the center of the rectangle. Then add constraints (e.g. two length constraints of same size) to make it a square.
Close the sketch editor.

Second step:
Copy & Paste the created sketch. Select the second sketch and go to Edit > Placement. Inside this panel define the rotation axis to be (1,1,0) and use an angle of 90 degree.

Now you already have the six points you need for the octahedron.

Third step:
Go to Part and use the command Shape Builder. Here add the additional four edge you need.

Fourth step:
Now create the eight faces from edges. This is a bit a click work. In order to be able to pick an edge you have to hide the new created face.

Fifth step:
Select all eight face and create the shell

Sixth step:
Hide all faces and select the shell. Now select the shell and create the final solid.

Done.

[wmayer]

Try this, use a cube in wireframe display mode for construction, build the faces for half, from either Draft Line or Draft Dwire, then in Part Worrkbench Fuse, Mirror, Fuse, then convert to solid.

Hm, for a valid octahedron all edges should have the same length. However, this is not the case for the both objects.

[NormandC]

Hey guys,

Sorry to piss on your parade , but the problem with both your methods is that the result is not parametric. If you change the cube size in Mark's file, or the sketches size in wmayer's, the final object won't update; you need to start over.

Here's my take, it's fully parametric although two values need to be changed:

• The width of the construction equilateral triangle in Sketch under Pad;

  

  FC_Parametric_Regular_Octahedron_01.png (13.04 KiB) Viewed 3405 times

• The length of Pad needs to be set to the same value as in Sketch.

cubegoldberg, let me know if you require a detailed explanation.

[wmayer]

Norm = but it's a pretty clever way.

Btw, another way would be to construct the top and bottom points and then use the loft tool.

[Robocut]

Norm = but it's a pretty clever way.

Btw, another way would be to construct the top and bottom points and then use the loft tool.

Can this be done such that changing a parameter will cause it to update correctly?

[quick61]

Try this, use a cube in wireframe display mode for construction, build the faces for half, from either Draft Line or Draft Dwire, then in Part Worrkbench Fuse, Mirror, Fuse, then convert to solid.

Hm, for a valid octahedron all edges should have the same length. However, this is not the case for the both objects.

Quite right.. oops - we'll say it was not enough coffee today.

Try this one.

Octahedron1.png (27.8 KiB) Viewed 3398 times

Octahedron_Fixed.fcstd

(21.08 KiB) Downloaded 76 times

No mirror, just fused faces from Dwire.

I see Normand posted during my redo. Your right Norm, mine is not parametric. (and why would I ever be upset over being shown a better / different way to get a task done? )

Mark

[bejant]

Greetings cubegoldberg, I guess you can see the answer is usually not to do the calculations unless you have to - let FreeCAD do them for you instead. To rotate a plane, first create a plane (or Sketch). Select it in the tree view, at the bottom of the tree view click the Data tab, double click the 3 dots to the far right of the Placement property to open the Placement dialog window, and change the position as needed. You can toggle "Apply incremental changes" to True and see the changes occur as you change the values.

Post back if you need more help or it's not clear.
======================
Nicely done Norm!
I used the improved measurement tool on 1/4 of your model and really like the increased functionality:

20140723a_octahedron.png (10.76 KiB) Viewed 3392 times

[NormandC]

Norm = but it's a pretty clever way.

Btw, another way would be to construct the top and bottom points and then use the loft tool.

Thanks guys

I was actually inspired by ulrich1a, who uses construction geometry in sketches in a much cleverer way than I. His geodesic pentagon is awesome.

I didn't even think of using the Part Loft tool! A Draft Rectangle and a Draft Point would be all that would be needed to make a pyramid, then mirror it.

Can this be done such that changing a parameter will cause it to update correctly?

No, you would need to manually change the Z height of the point, and that would require you to calculate its correct Z coordinate.

With my method, you don't need to.

guess you can see the answer is usually not to do the calculations unless you have to - let FreeCAD do them for you instead.

I wholeheartedly agree with that! I hate having to get the calculator.