How to create a joined part

Can anyone explain how to do that?

When following the help "Creating a Joined Part" I can't get to the point
where "join" is active in my menu Insert - Features - Join

Please be very specific if you give directions...

 

Follow the help file. It expalins it all right there. You just have to
remember to exit the sektch to make the join work.

Heck I'll just post it for you:

To join parts:

1) Create the parts that you want to join, then create an assembly
containing the parts.
2) Position the parts as desired in the assembly. The parts may either touch
each other or intrude into one another.
3) Save the assembly but do not close the window.
4) Insert a new part into the assembly:
a) Click Insert, Component, New Part.
b) Enter a name for the new part and click Save.
c) Click a plane or planar face on a component on which to position
the new part.
d) Exit the Sketch
5) Click Insert, Features, Join.

The Join PropertyManager appears.

6) In either the FeatureManager design tree or the graphics area, click the
components you want to join.

The names appear under Parts to Join.

7) Select the Hide Parts check box to hide the original components after the
join is complete.
8) Select the Force Surface Contact check box if you want to join any
coincident faces (as well as intruding volumes).

The software finds the affected faces, then extends the face with the
smallest area into the other component, and fills in any resultant gaps.

9) Click OK to create the joined part.


"d)" is the missing bit of information that you need to complete a joined
part.

Regards,
Scott

 

another alternative, you could create a new part (empty) and insert the
other parts and "combine".

 

Well, it still doesn't work...

somehow I dont get a sketch.... when I insert new part I pick my standard
template (...maybe thats what makes it wrong..?), then I pick a face and
then my existing parts get into this "transparent line state" - but there's
no sketch.

I am realy trying to simplify a very huge assembly - I would like it to be
reduced to a simple solid component that loads faster - and I thought that
was the way by joining all parts. But I would like to be able to do that
based on the big assembly - and not having to build it all again in order to
join parts.

The assembly has app. 5000 parts and takes 10 minutes to load....

 

Just save your assembly as a part. That would load it faster

Regards,
Scott

 

Tried that - but I get this 55 MB part.

unless I can reduce it to just the outer surface I guess I dont gain
anything in performance.

 

Steve,

So,...you... Edit Assembly; Insert/Component/New Part;... click on a
face? (I'd suggest clicking on the first default assembly plane),...
then.. make sure you click on the "Rebuild" (red/green light) button and
then,.. you have the Insert/Features/Join?
Otherwise,.. Edit Assembly again and RMB (right mouse click) on the new
part and check to see if Insert/Features/Join is there now?
It should be there?
Anyhow, you should be able to use the fly out (Show Feature Manager)
(click on "Join" bar, top of menu), then shift select all of your parts
to include in the "Parts to Join" list.

Otherwise, as Scott suggested, "Save as" a *.sldprt. It's not
associative, dumb solids/surfaces, but it will be one file. (wish there
was a insert part option to save all as inserted or join parts?)

...

 

I have just come up against this complexity overhead the other day, putting together a big conveyor layout half the size of a football field. Each conveyor has alot of parts.
What I would like to do is create a simplified, medium sized, assembly B, for insertion into an even bigger assembly A, but also have A update if any changes are made in B.
Sort of like the next level of model intelligence up from creating a completely dumb solid (parasolid export/import), but not completely full of all the mates/relations etc that is in a regular assembly.

Does anyone do this on a regular basis, can it be achieved with the SW as it stands now.

 

What option did you pick when saving it as a part?

You get three options:

1) Exterior Faces = to save the exterior faces as Surface Bodies .
2) Exterior Components = to save the visible components as Solid Bodies .
3) All Components = to save all components as Solid Bodies .

NOTE: Components that are hidden or suppressed are not saved when you select
All Components.

You should pick option 2 or 3 to get the lowest MB part file. - IMO

Regards,
Scott Baugh, CSWP

 

I just ran across the same thing a few minutes ago (before checking
the NG messages).. The "Insert", "Feature", "Join" is available in the
PART menu, not the assembly menu.

I ended up throwing in a dummy sketch to get the part to show
In-Context, then
once it was showing, the part menus (and therefore the "Join" feature)
was available. Kind of an 'egg before the chicken' type of thing

 

my alternative method was referring to "combine" not "join"

 

Just save the assembly as a part.

 

Hi Dale,
So far that's about the only way I can see to do this,
an awful amount of fannying around tho' when there are alot of parts.