Turning an Assembly into a part

Is it possible to create a drived part from an assembly?
When creating the gearbox case which is fabricated I create the weldment as
one configuration then I do all the machining operations in a new config.
I'm thinking that by keeping this as an assembly it will slow SW down when
incerted as a sub-assembly. Thats why I want to create a part from the
weldment assembly but I want the part to update if changes are made to the
weldment.

 

You...could...use the Join Command. This takes an assembly and joins it
into a single part...BUT all parts in the assembly must touch or
interfere. Usually, there are some problems with using the join
command.
BESIDES, this will not really speed up your model anyway. In fact, it
will most certainly slow it down.

My Suggestion:
If you just want a way to insert this gearbox assembly into another
assembly with a minimal performance hit, I suggest using a simplified
configuration. Just make another config of your gearbox assembly that
suppresses all unnecessary stuff. Then insert that simplified config
into your new assembly.

 

Nathan,

Check out the "join" feature in the help section. I think is what you are
looking for. You can take any assembly of parts and "join" them into one
part. The joined part is fully associative to the original parts.

Hope this helps
Rob

 

You can also do a File-> Save As on the Assembly and Select part from
the File Type Pulldown. This will let you save a n assembly as a
multi body part file.

Todd

 

If you want a little assistance with joining, I can send you the article I
wrote on the subject. Let me know.

WT

 

But this is not associative with the original assembly file. If the
assembly changes, the 'Save As Part' file will not update.

It does provide a nice performance boost, however.

 

We added a script to our PDM that automatically creates the Part from the
Assembly to solve the synchronization problem.

 

You can also do a File-> Save As on the Assembly and Select part from

Hmmm. Interesting idea. I am curious, though. If you use the 'Save As
Part' in another assembly and mate to it, do the mates loose their
references when another version is 'Saved As Part'?

 

You should be able to do a "Replace Part" or perhaps even ovewrite the old
file with the new. Broken mates will probably be an issue depending upon how
many topographical changes were made. The "Repair Mate" tool is pretty good
though.

JJ

 

The references remain intact - unless you do something to that feature that
would break them anyhow. When you save an assembly as a part, you wind up
with all of the former parts as distinct bodies in the assembly. Those
bodies retain their features, so there aren't any problems with mating. You
cannot, however, replace the assembly with the part (or vice versa) and have
the mates work out.

 

Using the save as assembly as part route, obviously any changes in the
assembly are not reflected in the part file unless a macro is used to
keep the part file up to date as suggested by Gabe. However I find
that the mates can broken to a point where they are difficult to
diagnose occasionally.

What would be nice is if a face could be give a unique name that will
remain constant regardless of other changes to the model (provided the
face in question is not altered). Now this is possible using the
'RC/Face Properties/Entity Information' box but this seems to have no
effect on mates.

A new idea I am going to trial (as time permits) is to create 0 offset
surfaces of critical features, (bosses, holes, etc which will be used
in the assembly for mating purposes). Then hopefully applying mates
to the surfaces rather than the solid faces will allow mating surfaces
to be preserved regardless of any changes to the model. This of
course relies on the 'hope' that the surfaces won't be renamed... okay
I'm probably clutching at straws.

Regards
Iain

 

Iain,

A word of caution.... I have played with using surfaces in the same way.
The biggest drawback I found with them is if you ever want to use those
surface models in a drawing. SW won't play well with surfaces in drawings.
Try to create a dimension in a drawing to a surface (not a face), and you'll
see what I mean. I have gotten it to work before - sort of - by creating
sketch segments to represent the surface that the dimension would reference,
but it is a REAL pain.

 

I've still haven't decided on what I should do, I've been doing alittle bit
of playing around. The one problem I am having is when I insert the assembly
with the sub assembly of my weldment into a drawing and I create a section
view, my case is hatched as different parts and you can see all the
different parts of the sub assembly (weldment).I want it to look like all
one peice hide lines all hatched the same. I run into a similar problem when
I create a part from my weldment assembly, the cross hatch is right but I
can still see the line where my parts join in my assembly. The line wont
goaway when I RMB "Hide Edge"

Thanks for all your help guys

Nathan Feculak

 

Wayne,

If it's not too much trouble, I would love to read what you have on
joining, as well.

Sincerely,
Jerry Forcier

 

We design mobile mining equipment and a majority of our assemblies are
fabricated and than machined. The machining operation is a
configuration that uses assembly cuts. This method works well for us
and theres no noticable slow down caused by using assebly cuts. We
prefer this method because it keeps the designer focused oh how the
assembly is actually made and less on how to work around the system.

 

This is curently what I do as well but the problem that I have is when I
section the view my sub assembly of my case looks like 10 different part and
I need to show it as one. For some reason when I try to hide lines they wont
hide, and I would like to crosshatch them as one peice.

Nathan

 

To change all components in an assembly section view to the same
hatch. Right mouse click on a cross hatch select properties, pick a
hatch style, and select apply to "view" this will change all
components to the same hatch.