OBELISK
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OBELISK
Hi to everyone and thank you for your time. How can I obtain an obelisk by creating a pocket on two faces of a parallelepiped, but not obtaining what I have on my screenshot?
I am quite sure there is a problem of dependency and probably I should use other systems such as loft for example.
Please your help will be really appreciated !!!
OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6712 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: da2d364457257a7a8c6fb2137cea12c45becd71a
Python version: 2.7.11
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
I am quite sure there is a problem of dependency and probably I should use other systems such as loft for example.
Please your help will be really appreciated !!!
OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6712 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: da2d364457257a7a8c6fb2137cea12c45becd71a
Python version: 2.7.11
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
Re: OBELISK
The approach in FreeCAD 0.16 will be a helper pad. This allows to attach the pocket sketch to the right place. The helper pad will be than removed by the pocketing action.
Ulrich
Ulrich
- Attachments
-
- obelisco_helper_pad.fcstd
- (25.9 KiB) Downloaded 44 times
Re: OBELISK
A good exercise for practising FC for myself also!
Alternative approach with 2 sketches + expressions in spreadsheet, so the form can update according to input in the spreadsheet field.
Hope other have another approach to learn more
In fact, the mathematical formula (almost forgotten since high school) take me more time, and NormandC's hint below help the top part.
https://forum.freecadweb.org/viewtopic.php?t=4230
Alternative approach with 2 sketches + expressions in spreadsheet, so the form can update according to input in the spreadsheet field.
Hope other have another approach to learn more
In fact, the mathematical formula (almost forgotten since high school) take me more time, and NormandC's hint below help the top part.
https://forum.freecadweb.org/viewtopic.php?t=4230
Re: OBELISK
Here you go. My favorite approach for such parts is the draft clone method.
1. Make a side-view sketch of the part.
2. Pad the sketch symmetrically in the Part-Design-Workbench (Be sure to pad it big enough.)
3. Create a Draft-Clone of the Pad.
4. Rotate the Clone by 90° with the Placement. (You have to choose the correct axis!)
5. Make a common of both in the Part-Workbench.
Ulrich
- Attachments
-
- obelisco_draft_clone.fcstd
- (10.65 KiB) Downloaded 50 times
Re: OBELISK
Apparently this is a cleaner method! Thank for sharing!ulrich1a wrote: ↑Sat Sep 02, 2017 2:26 pmHere you go. My favorite approach for such parts is the draft clone method.
1. Make a side-view sketch of the part.
2. Pad the sketch symmetrically in the Part-Design-Workbench (Be sure to pad it big enough.)
3. Create a Draft-Clone of the Pad.
4. Rotate the Clone by 90° with the Placement. (You have to choose the correct axis!)
5. Make a common of both in the Part-Workbench.
Ulrich
-
- Veteran
- Posts: 2611
- Joined: Tue Feb 21, 2012 8:07 pm
- Location: Torino - Italy
Re: OBELISK
Very simple procedure
- Create a Pad with Sketch001
- Cut Pad from Pocket
you can complete with expressions in spreadsheet
- Create a Pad with Sketch001
- Cut Pad from Pocket
you can complete with expressions in spreadsheet
Re: OBELISK
I had some difficulties with loft during creating a obelisk...
I had created 2 sketches but was unable to select the sketches for the loft. When preselecting i get an error!!
OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.11575 (Git)
Build type: Release
Branch: (detached from e3066d1)
Hash: e3066d1424a96ee16845f700154b3f7c8f51bb9f
Python version: 2.7.13
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.1.0
I had created 2 sketches but was unable to select the sketches for the loft. When preselecting i get an error!!
OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.11575 (Git)
Build type: Release
Branch: (detached from e3066d1)
Hash: e3066d1424a96ee16845f700154b3f7c8f51bb9f
Python version: 2.7.13
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.1.0
- Attachments
-
- Obelisk.FCStd
- (14.08 KiB) Downloaded 38 times
-
- Screen Shot 2017-09-02 at 19.02.40.png (22.57 KiB) Viewed 2037 times
-
- Screen Shot 2017-09-02 at 19.02.10.png (58.71 KiB) Viewed 2037 times
Re: OBELISK
@renatorivo Brilliant solution, as usual from you.
@bee jee I believe Mac users have some more problems unfortunately. I got crashes from a simple sweep then I passed the file to my friend with WIN 7 and the sweep went fine.
@bee jee I believe Mac users have some more problems unfortunately. I got crashes from a simple sweep then I passed the file to my friend with WIN 7 and the sweep went fine.
Re: OBELISK
Another alternative simply with lofts + 2 sketch + 1 point - as attached.paullee wrote: ↑Sat Sep 02, 2017 3:02 pmApparently this is a cleaner method! Thank for sharing!ulrich1a wrote: ↑Sat Sep 02, 2017 2:26 pmHere you go. My favorite approach for such parts is the draft clone method.
1. Make a side-view sketch of the part.
2. Pad the sketch symmetrically in the Part-Design-Workbench (Be sure to pad it big enough.)
3. Create a Draft-Clone of the Pad.
4. Rotate the Clone by 90° with the Placement. (You have to choose the correct axis!)
5. Make a common of both in the Part-Workbench.
Ulrich
(All could be 'linked' via spreadsheet)
Now, I am not sure but there should be some criteria/scenarios for choosing between options by Boolean Common of 2 solids or Lofting
It may depends on availability of information / design e.g. a section, subsequent ease of modification etc.
Re: OBELISK
In that case i ask on the developer forum.