[SOLVED] Cannot continue adding cylinders

[otto9F9otto]

My FreeCAD is acting in a bizarre way. I constructed a circle of tilted circles. I surrounded 4 of them with a cylinder and a subtractive cylinder in the middle, all shown in the screenshot. I want to do the same to all (40) circles. But when I add a cylinder to any other circle, my existing cylinders jump away. I also uploaded the file because this is so bizarre.
OS: KDE Flatpak runtime
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.14555 (Git shallow)
Build type: Release
Branch: (HEAD detached at 783e134)
Hash: 783e1346c7a078f5265c3f0c6a927d09a8c1fe70
Python version: 3.7.4
Qt version: 5.14.2
Coin version: 4.0.0
OCC version: 7.3.0
Locale: English/United States (en_US)

[freedman]

If you will want those cylinders to not touch when your done then you need to use the Part workbench, currently they touch, what is your goal? PartDesign needs to have one continuous solid.

[otto9F9otto]

The end result, freedman, is to have one continuous solid, exactly like what is shown. This will be fabricated via 3D printing, and will end up a part of a levitating top (magnets fill the holes).

So, are you saying that the Part workbench might be less likely to yield such bizarre behavior as I described?

[freedman]

I would use Draft array, it is an amazing tool. If you watch some youtube stuff you can learn how to use it. The attached I just threw together to give you an idea.

[quick61]

The end result, freedman, is to have one continuous solid, exactly like what is shown. This will be fabricated via 3D printing, and will end up a part of a levitating top (magnets fill the holes).

So, are you saying that the Part workbench might be less likely to yield such bizarre behavior as I described?

The way I would do it is to make a single hollow cylinder, (pipe), in Part Workbench and then use Draft > Array with the Fuse option enabled. Attached file is not to your scale, and is only intended as a demo of how it is done. Notice there are only 2 cylinders and the array...

Array40.png (34.55 KiB) Viewed 1433 times

Mark

array40.FCStd

(33.34 KiB) Downloaded 59 times

[Bance]

Is this what you are trying to achieve?

tiltedcircleBance.jpeg (61.41 KiB) Viewed 1426 times

You can change the angle like this:-

Screenshot from 2020-05-06 18-05-23.png (245.13 KiB) Viewed 1426 times

EDIT too late!

[otto9F9otto]

Yes, Bance, that is exactly what I am trying to achieve. Wow, you finished where I had to leave off. Thanks!

[TheMarkster]

There are always lots of ways to do things in FreeCAD, some better than others. Mine is not the best way, but an alternative. I created a Tube in Part workbench with inside radius 2.98mm, outside radius 4.2mm, height 4mm. I selected all the Edge objects and made a compound of them. Then ran this script to make Draft clones of each tube and attach them to the edges of the compounds since you had already gone through the trouble or rotating each of them. Final step was to fuse all the clones together.

Code: Select all

import Draft
comp = App.ActiveDocument.Compound
edges = comp.Shape.Edges
tube = App.ActiveDocument.Tube
for ee in range(1,len(edges)+1):
    clone = Draft.clone(tube)
    clone.Support = [comp,'Edge'+str(ee)]
    clone.MapMode = 'Concentric'

App.ActiveDocument.recompute()

Snip macro screenshot-f1fdc3.png (178.74 KiB) Viewed 1403 times

[otto9F9otto]

Way cool. Yes, another method to the same exact result. Thanks, TheMarkster.