Combining components into one part file

I regularly receive parasolid assembly files with a large number of
components. All of the components are supposed to be in one part (take
all the solids and combine them into one part to form the final part).
When I import the file into Solidworks, it creates an assembly file
with each component part in a separate file.

Is there any way to import the files into one part? Opening an empty
part and inserting each part works, but the parts don't come in in the
correct location and are a pain to relocate.

Alternatively, I can bring the geometry thru the assembly into a single
part file (using either the offset face with a 0.000 offset, or knit
the faces). But when I do this, I have to select each face
individually. Windowing around the body doesn't work. Some of the
solids have thousands of faces, so this isn't pleasant either. Is
there a better way?

 

well don't you have an option to save an assy as a part in SW ?

 

Ok. I finally figured out how to do that - not very intuitive, but it
worked.

Any ideas on the second half of the question? This is something that I
do often.

 

Keep in mind that even though you save as a part, that part will still be
dependent on the sub-parts. To get around that, you can join all the parts,
then parasolid out, and bring back in. It will then be a simple, stupid,
imported part - no ties. Kind of a pain, but usually works. We do it all
the time with imported gearmotors.

WT

 

I am not sure what you mean about tied to the assy? the new part file stands
alone does it not?

 

and you have options about how the assy is saved as a part...

 

On further review, when doing this there is a strange quirk. All the
components are converted into surfaces in the new part, and any
surfaces that were completely touching other surfaces are gone.

 

Never mind. I figured that one out.

 

the great thing about living in NZ is that being upside down enables you to
see the world in a different way and think it is completely normal...
....and now I am going back to bed on an excessively frosty morning to rest
my brain :O)

 

The only setting sort of answer I can find is the hidden switch for
"Import multiple bodies as parts". It seems to imply it's a general
setting, not for a particular format. The default appears to be "off".
To get to it, go to file, open, then switch to iges or step, not
parasolid, and you will get an Options button. The button isn't there
for parasolid. I'm not sure if this switch affects parasolids, it
doesn't seem to.

good luck.

 

That's a handy tip Wayne. I've never thought joining in SW then exporting
out to parasolid.

I also use alot of geared motors. I've been unioning them in Acad before
importing in SW. Often I them have to export out to parasolid to remove
errors.

 

To select all your faces - enable face filter, turn on wireframe, box
select the whole thing. Tada!

 

This is a common enough thing here that a few years ago I wrote an article
on it, stepping through the process and explaining how to handle some of the
errors. We have a guy here that still pulls it out whenever he does it.
Let me know if you would like a copy.

WT

 

To select all the surfaces of a part turn on the selection filters. F5
toggles the 'Selection Filter' tool bar and F6 toggles the on/off state
of filters in general. Turn on surface filter. Change your display
to HLV or WireFrame and window select over the entire model. This will
select all visible surfaces. Since you are in HLV or WireFrame this
means ALL surfaces are visible. To verify you can switch back to a
shade mode and you will see all surfaces onall sides of the part are
selected. Wow after looking at a simple model in WireFrame I don't
know how I ever worked that way in AutoCAD with full checking fixtures
and still kept everything strait.

Regards,
Corey Scheich

 

CS,
I tried that. It didn't work either. I cannot window select
anything thru an assembly. I am using SW2006 SP4.1. Don't know if it
works differently in other versions.

 

Ed,

I am doing it successfully in 2006 sp 4.0 in an assembly with WireFrame
and Hidden Lines Visible

Regards,
Corey

 

Wait a second it only works if you aren't in 'Edit Part' mode.
Interesting.....

 

Well when all else fails write a macro to do it =D. This macro will
select all faces in a part or an assembly document. If you edit the
macro you will see that there are a couple boolean values at the top
you can toggle. The first one specifies only select visible bodies in
a part. The second one lets you select subassembly faces or only top
level assembly faces. The defaults are:
Part - select all faces regardless of visibility status
Assembly - select all faces including subassemblies.

The macro also handles faces generated by assembly features just fine.

Posted at http:\\209.123.84.162\solidworks

 

Mr. Who,
I downloaded your macro, but it won't run. Just give the following
error:

Something went horribly wrong with the macro.
Error Code: 0
Description:

I have never done any VB coding, so I'm not sure what's wrong. Any
ideas?

 

Yup, I uploaded the fixed macro. For those in api wondering what went
wrong - I forgot that VB always runs the last sub as the main function.
Such an annoying default behavior!!! I changed my subs to functions
with no return value and it runs fine now.