Make a 3D model from a dxf file

[arcol]

Damn shoogen, you just solved in an half an hour,
while I was on the problem for days!
Thank you!

It is general enough to be the preferred workflow for dxf files.

Although I have a problem.
When I open the dxf file, it imports partially, things are missing:

dxf_import_buggy.png (75.72 KiB) Viewed 1985 times

Now, how about remodelling the stuff using sketches?:)
I stuck with it too (I want to chew this problem from every angle).

I can not rotate the holes for example (with polar pattern feature)....

[NormandC]

Cool example, I'm sure one of the guys will suggest a Part Design workflow for it.

I would model half of it then do a Part Mirror and fuse the mirror copy with the original.

[shoogen]

You probably need to increase the Draft precision ("Internal Precision level") in the preferences.
BTW: I imported with all automatic joining disabled. I don't know if this makes any difference.

[jmaustpc]

In this specific case, turn off join geometry, either 1) import as Draft entities or 2) directly as a sketch

If 1) then multi-select all the Draft entities, then click Draft to sketch, they will all go into just ONE sketch.


Then go to PartDesign and just "pad" to thickness ....and it works.


If you want to be able to adjust things then start constrainting things. Firstly PartDesign menu....validate sketch ...finds the missing coincident constraints..... then click fix.

As to where to go from here ....you first have to decide what is your most basic important base point or aspect from which to define everything else.

Jim

[arcol]

You probably need to increase the Draft precision ("Internal Precision level") in the preferences.

Internal precision level: 6 (by default)
Dimension precision level: 2 (by default)

Increasing 6 to 7, makes the import function work as expected.

BTW: I imported with all automatic joining disabled. I don't know if this makes any difference.

By all the automatic joining, you mean "Preferences->Import-Export->Join geometry [ ]", can't find anything else.

If 1) then multi-select all the Draft entities, then click Draft to sketch, they will all go into just ONE sketch.

Not for me.
It will create (with this challenge file) 13 Sketches. So basically all closed loop results a single sketch file.

I can jump this hole with the pasted python script.

If you want to be able to adjust things then start constrainting things. Firstly PartDesign menu....validate sketch ...finds the missing coincident constraints..... then click fix.

Well, then after fixing the coincident constraints, i end up (with the challenge file) 89 degrees of freedom (153 by default).

I believe it is a no-go. And I think normandc advised against it just in this very same thread.
But anyway, here is a sketch with 34 degrees of freedom, after adding 84 constraints.

dxf_import_challenge_single_sketch.fcstd

(6.96 KiB) Downloaded 43 times

[jmaustpc]

BTW: I imported with all automatic joining disabled. I don't know if this makes any difference.

yes it does for me, with enabled...I get some duplicate shapes and Draft objects, when it is disabled the import worked fine.

When disabled a multi-selection of the Draft objects then Darft2sketch creates one single sketch

When enabled a multi-selection of the Draft objects then Darft2sketch creates many sketches

[arcol]

When disabled a multi-selection of the Draft objects then Darft2sketch creates one single sketch

For me it takes effect only if I restart freecad. (File->close all is not enough).

[jmaustpc]

When disabled a multi-selection of the Draft objects then Darft2sketch creates one single sketch

For me it takes effect only if I restart freecad. (File->close all is not enough).

You currently have to restart FreeCAD for changes in Draft preferences to take effect, every time you change a Draft Preference.

[quick61]

Reading through this, thought I'd just offer my take on converting 2D DXF to 3D solid. Raw FreeCADdemo DXF to Part

Mark

[arcol]

Reading through this, thought I'd just offer my take on converting 2D DXF to 3D solid. Raw FreeCADdemo DXF to Part

Thank you quick61 for the educational video, it is a yet another solution to the problem!

Now, I'm more wondering how to model this very same model in freecad.
I turned into one giant sketch -> Number of constraints just exploded to a point, I could not manage it.

dxf_challenge_single.png (245.36 KiB) Viewed 1930 times

Then I tried to turn the outline into a single sketch, pad it, then one hole, but when I wanted to rotate it
90 degrees, I could not reference it to the middle of the big circle.

So now I'm really curious how to model it in Freecad.