Carve / Rabbet Around The Edge of an Object
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Carve / Rabbet Around The Edge of an Object
Hello! I've designed a body with a moderately-complex outline, and now I'd like to create a uniform slot feature around the perimeter (in woodworking terms, a rabbet), similar to the feature already present along the inner edge (which was a simple circle sketch cut):
this post that describes the sort of thing I'm trying to achieve, but I get a bit stuck with chrisb's answer when it comes to the draft step.
Anyway, it strikes me that this is another operation that is very much like a fillet or chamfer, both of which end up calculating an inset path along the selected edges of an object. If I could take the calculated resulting edges of a chamfer and magically turn that into a sketch to then extrude a cut (or create a body to use in a boolean cut operation), my work would be done.
It's quite possible I've painted myself into a corner due to the approach I took in designing the part so far; FreeCAD provides numerous ways to accomplish the same goals, and I chose the workflow with which I'm most comfortable (Part Design). Fortunately the design isn't too awful complex, so if someone wants to suggest another approach that would make this easier, I'm all ears!
I've attached the file and here's my version into:
OS: Debian GNU/Linux bookworm/sid (XFCE/lightdm-xsession)
Word size of FreeCAD: 64-bit
Version: 0.20.25695 (Git)
Build type: Unknown
Branch: master
Hash: 582c26ea8b5f9d85957a6cb1bf798839fa2ce94c
Python version: 3.9.2
Qt version: 5.15.2
Coin version: 4.0.0a
OCC version: 7.4.0.beta
Locale: English/United States (en_US)
Thanks for any and all suggestions!
I found Anyway, it strikes me that this is another operation that is very much like a fillet or chamfer, both of which end up calculating an inset path along the selected edges of an object. If I could take the calculated resulting edges of a chamfer and magically turn that into a sketch to then extrude a cut (or create a body to use in a boolean cut operation), my work would be done.
It's quite possible I've painted myself into a corner due to the approach I took in designing the part so far; FreeCAD provides numerous ways to accomplish the same goals, and I chose the workflow with which I'm most comfortable (Part Design). Fortunately the design isn't too awful complex, so if someone wants to suggest another approach that would make this easier, I'm all ears!
I've attached the file and here's my version into:
OS: Debian GNU/Linux bookworm/sid (XFCE/lightdm-xsession)
Word size of FreeCAD: 64-bit
Version: 0.20.25695 (Git)
Build type: Unknown
Branch: master
Hash: 582c26ea8b5f9d85957a6cb1bf798839fa2ce94c
Python version: 3.9.2
Qt version: 5.15.2
Coin version: 4.0.0a
OCC version: 7.4.0.beta
Locale: English/United States (en_US)
Thanks for any and all suggestions!
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- Mega Hex Par Gel Faceplate.FCStd
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- thomas-neemann
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Re: Carve / Rabbet Around The Edge of an Object
The original is a PartDesign model. So you should try - and it is easy here - to stay in PartDesign. Models don't become better if you force them to be non parametric. Besides: you added an unconnected origin plane somewhere.
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Re: Carve / Rabbet Around The Edge of an Object
Here is a PartDesign proposal. It is tedious to select all the edges, so I would propose a slightly different way of modeling: Make an own sketch for the outer loop. Then use this with a CarbonCopy to create what is now "Sketch" and use it later for the subtractive sweep.
- Attachments
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- MegaHex_cb.FCStd
- (124.22 KiB) Downloaded 23 times
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
- Shalmeneser
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- Location: Fr
Re: Carve / Rabbet Around The Edge of an Object
(Pocket(000) from your file is support by Face : Topological_naming_problem )
My way : work less for more result (1/4×4=1)
My way : work less for more result (1/4×4=1)
- Attachments
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- Mega Hex Par Gel Faceplate_SHALM.FCStd
- (266.84 KiB) Downloaded 19 times
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- Capture du 2021-12-03 19-39-43.png (32.93 KiB) Viewed 1398 times
- thomas-neemann
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Re: Carve / Rabbet Around The Edge of an Object
i can't find any difference to the original file. has the wrong file been uploaded?
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Re: Carve / Rabbet Around The Edge of an Object
1) Install WireFilter macro from tools menu -> addon manager -> macros (if you can get the addon manager working with the wiki -- otherwise search in the wiki for it and install manually)
2) Select Sketch and run macro, give it the okay to create the wirefilter.py file in your macros folder.
3) Select WireFilter object, and in property view in the "Wire Order" group set "Use Selected" to False. Edit Wire Order property from [1,2,3,4,5,6,7,8] to [8,0,0,0,0,0,0,0] by pressing the [...] button and putting 8 at the top line and deleting everything else.
4) Should now look like this on the screen with the WireFilter object shown and everything else hidden:
5) In the Offsetting group set Offset to -2 (for a 2 mm inset), and set Offset Fill property to True. Should now look like this:
6) Select the face in the 3D view and use the Pocket tool to create a 4 mm pocket, setting symmetric to plane checkbox to true. This pockets 2 mm in both directions. Alternatively, experiment with the reversed checkbox and do 2 mm for 2 mm depth. This is the view from the bottom of the pocketed object, with the selected face showing what was removed with the pocket operation:
Before the pocket, for comparison:
2) Select Sketch and run macro, give it the okay to create the wirefilter.py file in your macros folder.
3) Select WireFilter object, and in property view in the "Wire Order" group set "Use Selected" to False. Edit Wire Order property from [1,2,3,4,5,6,7,8] to [8,0,0,0,0,0,0,0] by pressing the [...] button and putting 8 at the top line and deleting everything else.
4) Should now look like this on the screen with the WireFilter object shown and everything else hidden:
5) In the Offsetting group set Offset to -2 (for a 2 mm inset), and set Offset Fill property to True. Should now look like this:
6) Select the face in the 3D view and use the Pocket tool to create a 4 mm pocket, setting symmetric to plane checkbox to true. This pockets 2 mm in both directions. Alternatively, experiment with the reversed checkbox and do 2 mm for 2 mm depth. This is the view from the bottom of the pocketed object, with the selected face showing what was removed with the pocket operation:
Before the pocket, for comparison:
Re: Carve / Rabbet Around The Edge of an Object
As mentioned by another responder, there seems to be no difference between your attached file and my original. Am I missing something?
TheMarkster's suggestion of WireFilter was a good one. Thanks for the step-by-step instructions, too! For some reason, Addon Manager is missing from my FreeCAD UI, so I had to install the macro manually. I was also missing some Python3 packages, which might be why the AM is missing in the first place. UPDATE: Yep, now it shows up.
To all, thanks a lot for the responses so far! This is a great community, and I'm glad to be a part of it.
Re: Carve / Rabbet Around The Edge of an Object
Sorry, I replaced the file in the post above.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.