convert 2D dxf file into 3D solid model

Hello,

The company Melles Griot provides 2D .dxf drawing files for its
opto-mechanical parts. I want to be able to see how the parts fit
together in a Solid Works assembly before purchasing them. I'm trying
to import the dxf files into Solid Works, but they remain as 2D
drawings (with multiple layers and colours). Does anyone know if I can
somehow convert a 2D .dxf drawing into a 3D solid model (.sldprt file)?

Thanks,

Dr. Zaius

 

If you have SolidWorks check out the helpfile
<2D to 3D Conversion Overview>

If not here's it says (briefly)...............

The 2D sketch can be an imported drawing, or it can be a sketch
constructed in SolidWorks. In either case, it must be a single sketch
in a part document.

NOTE: Even though the sketch can be an imported drawing, it must be
imported into a sketch in a part document. You can copy and paste the
drawing from a drawing document, or you can import the drawing directly
into a 2D sketch in a part document.

The conversion procedure is generally as follows:

In a part document, import a drawing into a sketch or construct a new
sketch.

Edit the sketch.

Extract sketches for views from the Front, Top, and so on. The sketches
fold up into the appropriate orientation.

Align the sketches.

Extrude the base feature.

Cut or extrude other features.

Kev

 

Ok, thanks for the info. I found the help file and tried to follow the
instructions. But I got stuck at the "Extrude the base feature" step.
It may be that the part is too complicated to do this. Can someone
please look at my .sldprt file to for me? I don't have any experience
with this sort or thing, and I'm not sure if I should spend a whole lot
of time converting many of these files. Maybe I should instead just go
to another supplier (ex. Newport) who provides the 3D files. If anyone
is interested, I can email you my .sldprt file. It's 535 Kb. And maybe
you can tell if it will work or not.

Thanks,

Dr. Zaius

 

I'll take a look. If I feel charitable enough
I will make the model.

Also send original DXF.

What version of SW are you working in?

 

Give a man a fish and he comes back for more.
Give him a fish hook and he can feed himself.

This is not that difficult and the upside to a little practice time is
that you will feel confident to get parts from the best source not the
source with the easiest geometry.

It takes a bit of practice to do 2D to 3D well. First of all you have
to make sure that the imported geometry is extrudable. There is a
TOOLS/SKETCH TOOLS/CHECK SKETCH command that will sometimes help with
this. Second, simplify, don't try to extrude the whole thing at once.
You can make multiple sketches from the original. Convert just the
outline and extrude first, then the holes, etc. Third, besides align
there are other commands in TOOLS/SKETCH TOOLS like Move/Copy and
Modify that can be a big help in getting your sketches lined up.
Finally, use contours when extruding. This will allow you to pick
areas of the sketch that will work.

And if you screw up you can always back up or start over. That's the
beauty of SW in general.

 

I pulled in a Mells Griot part. So here is some more information.

The part I pulled in was a ball mount. The dxf file contained a half
section view and a bottom view. This is a bit of a challenging part
from the standpoint of print reading. A few pointers:

Don't import title block, dimensions, text or hatching. Mells Griot
seems to have pretty clean drawings and the layers are pretty self
explanatory. Eliminate as much superfluous information as possible.

Check a dimension or two after importing to make sure you got it in 1:1
and not inch or metric as the case may be.

Do import centerlines.

Only the section view lines need to be pulled onto the front plane.

Use the trim tool to trim back to the centerline on revolved parts.

Likewise use the extend tool as necessary. The objective is to get
closed areas that can be revolved.

Recognize that the dxf file may in fact be an assembly and not a single
part. Multi body is ideal when importing. Turn off merge features.

If an assembly, The split feature will allow you to export the separate
bodies as an assembly which can then be made movable.