How to Convert DWG/DXF file to a 3D SolidWorks file

2d to 3d conversion; autocad to solidworks file; dwg to sldprt; dxf to sldprt file

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Closed Caption:

hi my name is Tommy magani I work for
progression technologies i'm going to
show you how to import a dxf into
solidworks and make that into a 3d part
file so first I'm going to go to file
open and open this dxf file that i have
and i get prompted with this import
window and i'm going to choose the radio
button to import to a new part and i
want to i want the 2d sketch that's what
I'm going to start with is a 2d sketch
then I have some options in this
document settings window I'd like to add
constraints and then I can also select
layers so in this case I don't want the
title block I don't need that so I want
to de-select it so i'm going to go to
selected layers and I assume it's on the
format level but as you can see it
doesn't look like it if I d select 0
takes away all of it so I'm gonna have
to do that manually so we're gonna go
ahead and hit next and this is where I
can kind of zoom out and remove the
entities I don't want to import so I'm
just going to do rubber bands the leg
I'm just hitting the Delete key you can
also click on this button that says
remove entities
i'm also going to delete this isometric
view because I don't need that
not for this exercise okay I'm gonna
finish and when it says unable to
explode box blocks option i'm going to
say no so now i have a 33 sketches all
on the same sketch plane all on the
front plane but don't worry we're going
to fix that we're going to actually
designate each of these as the front top
and side view and solidworks going to do
some tricks for us so the first thing
solidworks will do is put this 2d to 3d
toolbar on there for you when you do
this exercise that automatically places
that toolbar if you don't see it you can
right-click on the command manager and
just select 2d to 3d and you'll see this
the very first button is the front plane
so it wants you to designate which item
is the front sketch so I'm just going to
select this item and click on the front
sketch button and you'll see that all
the entities turned in into a gray color
okay now all the other items have lit up
so that you can select the other items
and choose now the reason they do this
is they always want you to designate
what is the front plane first before you
continue so now I'll select this item
and designate it as the top
ok now left my Center mark lines from my
autocad drawing but don't worry about
that i'm just going to go ahead and
delete that later and then finally i'm
going to select these items and
designate that as the right sketch this
is really cool it just kind of flips
that geometry over for you so now you
can see that were were making progress
towards a 3d part
is quickly delete this now I'm going to
ctrl select two entities and make them
align with each other if you see this
you rotate you'll see that the sketch is
kind of out of position relative to this
top sketch so I want to align this back
face it'll be a face to this edge so I
just held control and i selected both
lines that i want to line up and i'm
going to choose this icon is a line
sketch and it just shifts it over for me
and I think everything else looks ok now
I'm going to exit the sketch and you'll
see we have three distinct sketches so
in this case I'm going to start with
sketch for and i'm going to start my
solidbody extrusion so use the the icon
that says convert to extrusion ok so it
understands what geometry we want to
extrude so this is where its tricky
you'll have to go to the from group box
and its own sketch plane we want to
choose from vertex now we can choose a
vertex to start i want to start the
extrusion here and then I want to end at
this vertex ok so this is probably
starting to make sense the nice thing
about this is that you get the immediate
preview so you know whether you're doing
this right or not so I'm going to go
ahead and right-click and click ok and
as you can see i have a solid body and
you can just kind of rotate it just to
do these checks and you'll see that your
existing sketches overlap in the right
place
ok now we need to cut that hole through
this top face that's also easy to do I'm
going to pre-select
this circle and just select convert to
cut and we can choose a surface if we
like now that we have a solid body we
can choose surface and then we can
choose up to next and that looks right
to select ok ok so now we have a 3d part
it looks exactly like what I wanted it
to and you can just do a visual check
just by doing a normal to view and these
existing sketch lines should overlap in
the right place
it's just like a visual check and of
course you don't want to see these
sketches after you've created your solid
body so I like to right-click and hide
right click hide and you have a really
nice 3d part now you can save it and
create an assembly using this part I
magani thanks for watching our tech tip
video