Convert iges 3d surface to part

[vinot]

Hello everybody,

I'm trying to convert a 3d nurbs surface (iges format) to a solidworks
surface in order to process it, so it means that imported surface must
be "workable".

When I import the file with Solidworks I obtain an "imported" surface,
wich not allows to be modified, ie. copy some sketch over the surface.

If I try to do it with 3d points, importing a 3d dxf, I obtain a point
cloud but all within one plane, so importing 3d dxf seems don't work
well.

Any suggestion?

Thanks in advance,

toni

[POH]

I assume that the objective is to modify the imported surface, so I'll
suggest the following:

1. Select the imported surface in SolidWorks and then Insert/Boss,
Base/Thicken (via the main menu) to create a solid body. (If the
imported data provides a set of surfaces which can be knit together to
create a closed volume, then a solid can be generated as an option
during the knitting operation. Also, surfaces can be created within
SolidWorks and added to the set of imported ones to complete the
closure.)

2. The solid body can then be modified using the Insert/Features/Scale
(or Shape, Deform, Indent, Flex, etc.) Once such features are added,
they provide some control for editing which can be considered as
parametric.

3. After modification, the resulting surface(s) can be copied (within
the part file) or exported, if desired, as separate from the solid.

Have a look at SolidWorks Help for information on the tools available
for modifying surfaces directly (such as trim, untrim, extend, move,
etc.), but these won't provide the sort of control you seem to be
looking for.

There are third-party Add-In programs available for SolidWorks to give
tighter controls over surface "push-pull"; however, to accomplish that
sort of thing within SolidWorks itself, it's necessary to first use the
surface(s) as the basis for a solid object.

Per O. Hoel
_______________

There are
That70sTick wrote:

Do you actually need the surface to change? Or are you just hung up on
the fact that it has no parameters to change?

If you need the surface to change, create a new surface in SW using the
imported one as a template. I do this on the Vellum-generated surfaces
supplied to me by our customer. Most of the time they are simple
sweeps.

Can you post the original IGES to http://www.mcadforums.com

[That70sTick]

Do you actually need the surface to change? Or are you just hung up on
the fact that it has no parameters to change?

If you need the surface to change, create a new surface in SW using the
imported one as a template. I do this on the Vellum-generated surfaces
supplied to me by our customer. Most of the time they are simple
sweeps.

[Sporkman]

vinot wrote:

Hello everybody,

I'm trying to convert a 3d nurbs surface (iges format) to a solidworks
surface in order to process it, so it means that imported surface must
be "workable".

When I import the file with Solidworks I obtain an "imported" surface,
wich not allows to be modified, ie. copy some sketch over the surface.

If I try to do it with 3d points, importing a 3d dxf, I obtain a point
cloud but all within one plane, so importing 3d dxf seems don't work
well.

Any suggestion?

Thanks in advance,

toni

If you want surfaces, that's one thing. If you want a solid, that's
another. It sounds as though perhaps you are NOT selecting "Try forming
solid" in the Options of the File > Open dialog box, and perhaps that's
really what you want to do . . . it's not clear. Even after selecting
that Option, however, SolidWorks may not be successful importing to a
solid body. Try with and without B-Rep mapping (with B-Rep mapping is
preferable if it works, and if it doesn't it tries knitting surfaces
together to form a solid). Otherwise, if you really want surfaces, not
a solid or solids, try "Do not knit" if you want to be able to address
individual surfaces . . . if you select "Knit surface(s)" it will
probably end up as being one big surface that you can't Trim to itself
or modify easily. If what you are importing is really an assembly --
more than one part -- try selecting "Import multiple bodies as parts".

Use the Help files.

If these things don't give you what you want I recommend using one of
the myriads of translating service shops. It'll save you more than you
spend.

'Sporky'

[That70sTick]

POH:
Good ideas. I'll have to remember these.

[vinot]

Thank you all!

really I have only to work with surfaces, and what I really need is to
know the x,y and z position of several points from the points cloud of
the surface. This points are defined by another "part", wich really
only define the x and y position, and the z position is defined by the
imported surface.

I will try it again using the above helps.

Thnks again,

Toni

[Jerry Steiger]

Thank you all!

really I have only to work with surfaces, and what I really need is to
know the x,y and z position of several points from the points cloud of
the surface. This points are defined by another "part", wich really
only define the x and y position, and the z position is defined by the
imported surface.

You can use projected curves to project your x and y values on to your
imported surface, then make a point in a 3D sketch and constrain it to the
curves. Now you can measure the location of the point.

A quicker method would be to make split lines on your imported surface, then
measure the point at the corner. The disadvantage is that your surface is
now several pieces, but maybe that doesn't matter.

Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"

[vinot]

Thanks again,

finally I have my surface workable! using boss and thickness, but
should work well. Now the hint will be obtain easilly the z position of
each point automatically, because what really I need is only this
value. Will try with macros, but I don't know if this method could be
posible.

thanks again

toni

[skateboardkid]

you dont have to thicken surfaces if they are forming an enclosedc volume, just knit the surfaces togeather and the combined part shows up in the solidbodies folder.