How to create face from shape?

[nquantum]

I do import aluminum extrusion dxf file in 2D. File download from website. Purpose is to make face and extrude to 3D.
It can extrude but hollow inside, without face. I've try use upgrade shape in Draft workbench but nothing happen. Shape not join into 1-shape, it just like shape no close. I've no idea how to make face of it.

Please help.

[NormandC]

Please attach the DXF file or provide the link to download it.

Basically you need to create two faces: one for all the outer profile and one for the inner outline. Then you subtract one face from the other.

EDIT: forgot about the 4 "cross shape" holes inside and the 4 little rounded squares. You need to create 10 different faces.

Would be much easier to convert everything to a sketch using Draft Draft2Sketch.

[nquantum]

Here is link that I get the file also I've attach it. https://grabcad.com/library/60x60-8n-br ... -profile-1

EDIT: forgot about the 4 "cross shape" holes inside and the 4 little rounded squares. You need to create 10 different faces.

I understand hole for 4 cross shape, 4 little rounded squares. But what you mean by 10 different faces, from what I see only 1 face on top and 1 on bottom.

Would be much easier to convert everything to a sketch using Draft Draft2Sketch

I've tried convert to sketch already but don't know what next to do to make face.

[nquantum]

I select all sketches or few sketches in treeview and sketch>merge sketch also nothing happen. Just same result like upgrade. Don't know why, it should combine all shapes/sketches into one shapes/sketches is it not?

[oldmachine]

First, in my opinion, it would be far quicker to completely redraw it in PartDesign.

Having said that, it was easy enough to get it done this way - basically, clipping the file to 1/4 and using symmetry, as follows:

In PartDesign workbench:
Create a New ‘Part’
Add a Body to the Part.
Import your .DXF
Box Select 1/2 of the dxf lines, Delete them.
Box Select 1/2 of the remaining lines, Delete them.
* Now, you have 1/4 the of the shape *

In Draft Workbench:
Select the remaining lines, Convert Bi-Directionally to sketch.
Delete all the Shape lines from dxf (but, keep the new sketch lines).
Move the sketch lines into the Body (created above).

In Sketcher workbench:
Select all the sketch lines
Sketch>Merge sketches (in menubar)
Delete all the sketches of the lines but keep the new merged sketch.
Clip the lines that extend past the H & H axis and close them with a new short line.
* Now you have one sketch of 1/4 of the shape *

In PartDesign workbench:
Drag the new sketch into the Body label
Validate the new sketch (Find and Fix - will delete what’s no longer needed)

Now you have two options
1 - extrude and mirror the extrusions
2 - mirror the sketches and extrude as one unit.

I choose to mirror the Sketches as is more useful/friendly for this particular part)
Mirror as needed to get the final shape (of four quarters)
Now, extrude (Pad) it…

Bingo!

[EDIT] Why did I choose the use 1/4 and Symmetry? Because, so many lines take too long for regeneration/update and I don't like waiting

[nquantum]

Thank you! It work! Now I can make it. Do I need to flag this topic as solve anywhere?

Still couple of curiosity remain.
1. Why I import dxf file into draft workbench it have no face since it close line? My guess is it seem to close but it is not.
2. Also in draft workbench I can not upgrade into one shape? My guess is also it not close line/shape.
3. Why symmetry? Why not just import dxf and merge sketches then extrude? Please more detail explain. You said it too long for something what does it mean? From 1/4 then ymmetry it later will not same result?

When you use symmetry? You use in these 2nd way you tell me in sketcher before extrude right?
Sorry I seem newbie question I'm still new finish some tutorial try to learn thing here. Purpose of symmetry seem unclear for me now.

[oldmachine]

There are other methods of doing it - I showed my way. I primarily use PartDesign workbench and, when needed, I use other workbenches in the most minimum way to get what I need for use in PartDesign.

DXF are just lines.
Draft uses (and creates) just lines.

Need to convert lines into usable format - a sketch.

With a sketch, you have ability to use PartDesign, thus, can now Pad and Cut. (PartDesign uses sketches, not lines and shapes).

You don’t need to cut down to 1/4 - you can convert all the DXF lines and merge into one sketch. But, I prefer not clicking so many lines and waiting for updating.
So, 75% faster.

After you get a sketch, you can extrude (or cut) with it. So, the point is to get the DXF lines into a sketch.

Having a sketch of 1/4 of full shape means you need to create three more sketches and orient them for the full shape.
Mirroring a sketch is quicker than other ways (for me).
Results are the same.
You could merge all 1/4 sketches into One full sketch, if preferred… That is what the last sketch is (MirroredSketch002).

Others can explain Faces and details of workbenches...

[UR_]

There are other methods of doing it

If you have access to a computer, let him do the job

workflow:
- import dxf with these settings:

FreeCAD 0.18-000031.png (86.11 KiB) Viewed 2613 times

- select all shapes and invoke PartWB:Compound->make compound
- select Compound and invoke DraftWB:Draft to Sketch
- select Sketch and invoke SketcherWB:Validate Sketch
- at "missing coincidences" set tolerance to 0,45 mm (because smallest edges are 0,5 mm)
- - hit button [Find]
- - hit button [Fix}
- select Sketch and invoke PartWB:Make face from wires
- extrude it if you like

FreeCAD 0.18-000032.png (86.25 KiB) Viewed 2613 times

file:

60X60 8N.fcstd

(313.5 KiB) Downloaded 22 times

done with:
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.14210 (Git)
Build type: Release
Branch: master
Hash: d2f9ab6a111975fce69c7f29bf3b7ecb8673a2db
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: German/Germany (de_DE)

[oldmachine]

'UR' That's a good approach - was very quick and did not need to cut it down to 1/4...etc
The trick is to setup the DXF import as you indicated... (still prefer to extrude in PartDesign)

Thanks for the tip

[NormandC]

I understand hole for 4 cross shape, 4 little rounded squares. But what you mean by 10 different faces, from what I see only 1 face on top and 1 on bottom.

Why I import dxf file into draft workbench it have no face since it close line? My guess is it seem to close but it is not.

Draft can only create a face from a single closed profile. In your DXF, there are 10 closed profiles:

Outer profile

FC_nquantum_import_dxf_01.png (8.05 KiB) Viewed 2564 times

Inner profile

FC_nquantum_import_dxf_02.png (7.41 KiB) Viewed 2564 times

Small cross shapes

FC_nquantum_import_dxf_03.png (6.15 KiB) Viewed 2564 times

Rounded squares

FC_nquantum_import_dxf_04.png (6.29 KiB) Viewed 2564 times

So you need to create 10 faces. Then, you subtract the smaller faces from the larger one with the Draft Downgrade button. This acts like a Boolean Cut for faces. Only then will you end up with a final face to extrude.

Here's an example with simple Draft objects which are also faces.

FC_Draft_Downgrade_Face_Boolean_01.gif (156.19 KiB) Viewed 2564 times

Unfortunately, it is not possible to upgrade any of your DXF's shapes to faces, probably this is a precision issue. So you'll have to work with oldmachine's or UR_'s solutions.