convert 2D dxf file into 3D solid model

If you have SolidWorks check out the helpfile
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
Dr. Zaius wrote:

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
alphawave wrote:

I'll take a look. snipped-for-privacy@liquidschwarz.com If I feel charitable enough I will make the model.
Also send original DXF.
What version of SW are you working in?
Dr. Zaius wrote:

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.