2D to 3D conversion

I'm struggling a bit to understand the best way to convert a 2D DWG to
a 3D model using the 2D to 3D conversion method outlined in help. The
problem I run into is after I have extracted my sketches to represent
my front, top and right views, the sketches are automatically offset
making it difficult to extude. If I extrude the front sketch to a
point on a adjacent sketch (top or right) I'm left with material
between the intended sketches. Is there anyway to specify the
extrusion as following the perpendicular sketch? or do I need to
create new planes?

 

It sounds as if you are talking about things the 'Align' tool on the 2D to
3D conversion palette provides. Have you reviewed the Help file?

JJ

 

as I know, 2D to 3D conversion is not an easy and automated task. You can do
only conversion of basic primitives and not too sophisticated solids.

The best tool for such converstion is Bentley Microstation (? - or another
Bentley application ; I don't remember which).

 

if you extrude from more then one view with option "Merge result"
un-checked. then use the command combine on both views bodies "Common"
checked as the option. Combine is not on the tool bar as default.
tools\customize\commands\features\"Combine". what you are left with is
the intersection from 2,3,4,5,6.... views mabey. remember to measure
the dimensions that show up on the drawing to what is drawing in 2d.
somtimes its better to translate the writen drawing by looking at it.
If you are planning on making major changes to what was 2d when 3d.
but if the only need is to use it in an assembly and drawing. then 2D
to 3D conversion will do a good job.

 

JJ,

Believe me I have read what's in help several times. The Align tool is
used to define a planar alignment. The specific question I have can be
seen if you go into the help topic "2D to 3D Conversion Overview". At
the top of this article it has an "> Example" button. If you scroll
down to where you it says "Extrude the base feature" and shows a blue
solid being created - my question is how do you define the starting
plane for the solid when the profile (or sketch) is offset? The
profile in blue highlight is actually offset from what appears to be
the front sketch where the original data is. Do you have to create
this plane or can you offset extrude?

 

Steve,

When you extrude from the front view select a point in the top or
right view to start the extrude, then start the extrude command from
the 2D to 3D toolbar, select a point to end the extrude. I believe
this is what you are looking for.

Greg

 

Greg,

I am confident you know what it is I'm trying to do, but I need a
little more clarification:

1. Select the Front view sketch (this highlights the sketch)
2. Select Extrude from 2D ro 3D toolbar
3. The default option for Extrude 'Direction' is "Blind"
4. Select a point in the Top or Right view. This changes Extrude
'Direction' option to "Up to Vertex" - this isn't right though because
it's not offset from front sketch.

What Direction option are you using to be able to select a start
vertex and end vertex? I have tried every Direction option in the
Extrude PropertyManager. Are you holding down a Shift key or
something?

Thanks,
Steve

 

Greg or someone? Please Help!

 

The key, (and Greg's message does point this out), is to pick both the
sketch segments and the start point which resides on the other sketch before
choosing the extrude command. In other words, step 4 becomes step 2.

The SW Help has a section on this if you search on "Extruding in 2D to 3D"
and it includes an example.

Good luck.

JJ