How to put a wire in a body?
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Re: How to put a wire in a body?
Why are you complicating everything with PD bodies?
Are they really needed?
Could you not just use Part extrudes?
Are they really needed?
Could you not just use Part extrudes?
Re: How to put a wire in a body?
This seems to get me a bit further with a limited amount of mouse clicks:
1. Import both DXF files.
2. Draft / Upgrade to wires.
3. Draft / "Draft to Sketch" of everything together.
4. Part Design: Put the sketch into a body and pad it.
I can do this a few times more for milling at different depths. This is my best effort yet, but I'm open to a better workflow.
1. Import both DXF files.
2. Draft / Upgrade to wires.
3. Draft / "Draft to Sketch" of everything together.
4. Part Design: Put the sketch into a body and pad it.
I can do this a few times more for milling at different depths. This is my best effort yet, but I'm open to a better workflow.
- Attachments
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- Box_03.png (128.01 KiB) Viewed 593 times
Re: How to put a wire in a body?
Hi Pintuxgu, greetings to the Community!
To do it with "Draft" and "Part" in a matter of seconds, create the extrusion of the box, then import the shapes from the dxf, then create wires for each one (just use the multiple selection function "Box selection") then join the wires into a compound, extrude the compound and finally do a boolean cut (difference) operation between the box and the extruded compound.
Attached is the file created with the procedure described.
You can then obtain a Draft-"Facebinder" from the perforated face to be converted into Sketch with the "Draft to Sketch" function
- Attachments
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- Box_Draft-Part.FCStd
- (57.3 KiB) Downloaded 10 times
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- Box_Draft-Part.png (172.59 KiB) Viewed 583 times
Re: How to put a wire in a body?
Returning to the original question: You can add Draft objects to the Group property of a body. I have done so with three rectangles, which I had upgraded to wires and then to faces. These can directly be padded and pocketed.
- Attachments
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- bodyOnDraft.FCStd
- (30.04 KiB) Downloaded 5 times
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
- papyblaise
- Veteran
- Posts: 7998
- Joined: Thu Jun 13, 2019 4:28 pm
- Location: France
Re: How to put a wire in a body?
if I remember correctly, we already made a stand for Allen key a short time ago (3 or 4 months)
- Shalmeneser
- Veteran
- Posts: 9558
- Joined: Wed Dec 23, 2020 12:04 am
- Location: Fr
Re: How to put a wire in a body?
* New file
* File > Import : --.dxf
* Select all shapes
* Draft_Draft2Sketch
* repeat
* (you can suppress shapes)
* PartDesign wb
* New body
* Move sketches inside the body with the mouse
* Modify Map Mode to FlatFace
* Modify Support to XY_Plane
* Pad and Pocket
* File > Import : --.dxf
* Select all shapes
* Draft_Draft2Sketch
* repeat
* (you can suppress shapes)
* PartDesign wb
* New body
* Move sketches inside the body with the mouse
* Modify Map Mode to FlatFace
* Modify Support to XY_Plane
* Pad and Pocket
- Attachments
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- Krimptang_SHALM.FCStd
- (76.06 KiB) Downloaded 7 times
Re: How to put a wire in a body?
Just had dinner and read about https://wiki.freecad.org/Part_and_PartDesign
I noticed you can:
1. Import DXF in Draft.
2. Upgrade once (to wire) or twice (to faces)
3. Part Workbench -> Extrude.
With the result that you have multiple extrusions: But as what I understand from the Wiki, "Part" and "Part Design" have a very large overlap in functionality. And to not confuse stuff further for myself, I will switch back to the Part Design Workbench, as I have much more experience with that, and the Part Workbench does not have to seem much advantage for me.
I noticed you can:
1. Import DXF in Draft.
2. Upgrade once (to wire) or twice (to faces)
3. Part Workbench -> Extrude.
With the result that you have multiple extrusions: But as what I understand from the Wiki, "Part" and "Part Design" have a very large overlap in functionality. And to not confuse stuff further for myself, I will switch back to the Part Design Workbench, as I have much more experience with that, and the Part Workbench does not have to seem much advantage for me.
Re: How to put a wire in a body?
I'm very close now, also thanks to Shalmaneser's last post.
I have now imported all layers at the correct depth, padded the outside, and made pockets with all the others on their correct depths.
There are two thinks I do not know what they are or how they work:
* Modify Map Mode to FlatFace
* Modify Support to XY_Plane
I see that these are part of the Sketch, (and not of the body). I will have to study more to understand what those are and how to apply those properties effectively. I guess that not having proper references for your sketches leads into the "topological naming problem" and malformed objects.
Skipping these steps did seem to work (I hope it's not blasphemy).
I found it quite surprising that FreeCAD can now work with sketches with multiple objects in a single sketch, and you can make a pocket from all of them at the same time. This has been a long standing limitation in FreeCAD. Another detail is that once I have created a sketch from the imported DXF file, al the imported "shapes" can be deleted to clean up the document tree.
As for now, the result looks like: I still want to change some small things before I go to the Path workbench (that would be a separate topic). The main thing is that I now have a workflow that works.
I have now imported all layers at the correct depth, padded the outside, and made pockets with all the others on their correct depths.
There are two thinks I do not know what they are or how they work:
* Modify Map Mode to FlatFace
* Modify Support to XY_Plane
I see that these are part of the Sketch, (and not of the body). I will have to study more to understand what those are and how to apply those properties effectively. I guess that not having proper references for your sketches leads into the "topological naming problem" and malformed objects.
Skipping these steps did seem to work (I hope it's not blasphemy).
I found it quite surprising that FreeCAD can now work with sketches with multiple objects in a single sketch, and you can make a pocket from all of them at the same time. This has been a long standing limitation in FreeCAD. Another detail is that once I have created a sketch from the imported DXF file, al the imported "shapes" can be deleted to clean up the document tree.
As for now, the result looks like: I still want to change some small things before I go to the Path workbench (that would be a separate topic). The main thing is that I now have a workflow that works.
- Attachments
-
- Box_Part_Worbench.FCStd
- (502.14 KiB) Downloaded 10 times
Re: How to put a wire in a body?
Update: Going from imported shapes directly to Draft / Draft2Sketch as Shalmeneser suggests does work, but it leaves all the lines as separate entities. If you first update them to wires in the Draft workbench, then the ends have coincident constraints in the resulting sketch, and this results in less work when you want to refine the sketch further.
I am also a bit confused by the location of a sketch in the document tree.
According to:
https://wiki.freecad.org/Sketch
> ... Nevertheless, a Sketch can always be created by itself for any other purpose;
A sketch can be created directly (as a stand alone object) in the Draft workbench by the tool already mentioned.
When working in the PartDesign workbench however, a sketch must always be a sub object of a body. It does not allow you to create a sketch in the root of the document for example. This seems inconsistent to me.
I am also a bit confused by the location of a sketch in the document tree.
According to:
https://wiki.freecad.org/Sketch
> ... Nevertheless, a Sketch can always be created by itself for any other purpose;
A sketch can be created directly (as a stand alone object) in the Draft workbench by the tool already mentioned.
When working in the PartDesign workbench however, a sketch must always be a sub object of a body. It does not allow you to create a sketch in the root of the document for example. This seems inconsistent to me.
Re: How to put a wire in a body?
Nonsense this has always been allowed.
I like to be able to choose where my sketches are created.....Pintuxgu wrote: ↑Wed Mar 22, 2023 7:13 pm A sketch can be created directly (as a stand alone object) in the Draft workbench by the tool already mentioned.
When working in the PartDesign workbench however, a sketch must always be a sub object of a body. It does not allow you to create a sketch in the root of the document for example. This seems inconsistent to me.