My best guess, not having attempted to use 3D PDFs, would be to position the part in each of the traditional 3 basic positions. Front, side and top. Then, I suspect, when you import the PDF it will come in as three 2D drawings. From there you would have to open a new sketch and convert the edges of the part into that sketch. Following this you can do the same with the other two views on the appropriate planes. Now you have three sketches that may or may-not allow you to guess the depth to extrude the sketches to.
You see 2D sketches do not have the necessary information to fully determine a 3D part. Your best bet is to use the measure tool in 3D PDFs to gather the information to model the part from the ground up all in Solid Works. You will gain valuable experience and have a much more correct model when you are finished.
Why wouldn't you open the DXF in SW using import wizard, and then copy the sketches to front, right and top planes in SW? Then you could use extrudes/ cuts to model the part.
I often have to work from DXF's, and I find it's often easier to leave the imported geometry in reference sketches, then covert the entities I need into additional sketches that I use to create features.
If you have multiple section views, you could create planes to put each section view on, then use lofts etc. to connect. (it would probably be better to use extrudes where you can, but lofts might be the only option if the geometry is complex)
That is basically what I said to do. A little clearer maybe, but basically the same. However every time I have attempted doing that it has taken me longer to do that than just starting over has taken.
I was confused by what you said about 3d pdf's - did you mean DXF?
I agree that it's often quicker to start over - however, I'm usually working with funky shapes from graphic designers, so bringing in a DXF with a lot of splines, bad lines etc. is often the only option. I usually leave all that on one sketch, then create new sketches to work from by converting/ drawing over the stuff in the original sketch.
Maybe I don't know enough about 3D PDFs. Are you able to bring it into SW and rotate/ re-position it in SW? If so would you be able to use the import geometry functionality? If you are only able to bring in a 2D view and then re-position the part and bring in another view. then essentially what you are doing is bringing in separate sketches (I used the term DXF for that but it isn't technically correct and 2D sketch would be more accurate).
Your need for funky shapes from graphic designers is where I have the biggest concern about using this method as you will have difficulty matching the transitions between the two different planes. For something like this you may be better off doing like someone suggested earlier and making several section planes and creating a sketch on each plane then doing sweeps or lofts between the sketches.
However, if you have graphic designers making the shape for you, what software are they using? The 3d PDF might not be the best source for information. If they are using a program like Rhino that creates a point cloud you could import that cloud from the Rhino file into SW as surfaces and then thicken the surfaces. This is exactly what I had to do when I was forced to learn surfacing. It is a fun challenging new world of SW to step into.
Thanks for the interest, Jim. Our designers are using Adobe Illustrator (2D only). The specify depths, radii etc. with text callouts (i.e. "Blue area 100mm in front of white area", "Green swoosh with heavy round over", "Red swoosh wrapped around edge"). I convert Adobe file to DXF (SW cannot open AI files, although they say it can. Opening Adobe Illustrator File )
I use the import wizard to open the DXF as a sketch, clean up that sketch, then use that as my master. I them create features, using convert entities to grab the geometry I need from the original sketch. The graphic designers have e-drawings, and can look at what I have modelled. When they are happy, I create STEP file as well as drawings to send to the vendor, or create drawings for all the sheet metal parts, depending on how that sign is being built.
As a final check, I open a PDF drawing with Illustrator, and paste the front view on top of the front view the designer created, to ensure that all lines etc. converted correctly.
If you have any suggestions as to a better technique, I'd love to hear them, as I'm very new to SW. Here's a picture of the kind of stuff we make:
Normally when you start a new part and insert a dxf/dwg, you're asked the select a plane,
once you imported it normally the commandmenu "2D to 3D" will be floating somewhere on your screen.
You now can go into the sketch, select the view you want and dedicate it onto, for example, your front-plane.
you can now do the same for Right-view; Top-view, ...
After you dedicated all views, you can go into each sketch and use the "align sketch" command to align, for example, all start-points.
From here on you can use every sketch to build up your 3D.
Hope this was informative.
Use SW help menu for 2D TO 3D
dxf to import
Import dxf to SW
curser over geometry wanted as front view, click "add to front sketch"
curser over geometry wanted as side view, click "add to right sketch"
top view, "add to top sketch"
align any sketches that are misaligned
add extrudes and other features using newly aligned sketch geometry
for sheet metal parts use extrudes first, then convert geometry to sheet metal
extrudes allow geometry to be extruded from point to point using sketches as reference
I have learned something. This is much improved from what I have attempted to use.
"A couple of these DXF views are the sections of this part."
For section views, you could:
1)create blocks of those views
2)add those blocks back to whatever view they apply to (side, front, top etc)
3)rescale, rotate and position blocks as needed
I have used the 2D to 3D. But, most parts I find it easier and faster to start from scratch.
When we first got SWX I thought I would use this method like crazy since most of our old drawings were DWG's.
Then I realized, for most of our parts it could do it faster from scratch.
The simple parts were a no brainier - we just made them from scratch.
But when I tried the more difficult parts that this would have been easier - I found that the dwg's were not always drawn correctly (lines not connected, dimensions off a little, elements roughly drawn in and then dimensions typed in instead of using real dimensions...)
In the end, I used the import method less than a dozen time and haven't used it at all in the last few years.
But now, we have a lot of dwg's that we know are correctly drawn and I have been looking at going back and trying this again.
Lots of great suggestions! Thanks guys! That 2D to 3D looks promising. I have used other CAD systems, where I could move or reposition the geometry. So, it's getting away from that method to use SW method is taking some time. But, I see how you all are doing it, and each method has it's merits.
I appreciate everyone's help.
..Another option, which I use often,.. Insert > "Derived Sketch"
..import your "sketch1"... exit the sketch1... cltrl select sketch1 and plane (or face or whatever) and Insert > "Derived Sketch"