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...
Reply to
steve
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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
Reply to
Scott
another alternative, you could create a new part (empty) and insert the other parts and "combine".
Reply to
kenneth b
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....
Reply to
steve
Just save your assembly as a part. That would load it faster
Regards, Scott
Reply to
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.
Reply to
steve
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?)
..
steve wrote:
Reply to
Paul Salvador
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.
--=20 Neville Williams (remove the "knot" to reply)
- I would like it to be
Reply to
Nev Williams
Have you looked at using simplified configurations, with things like fasteners and o-rings and other hardware suppressed?
Reply to
Dale Dunn
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
Reply to
Scott
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
Reply to
rocheey
my alternative method was referring to "combine" not "join"
Reply to
kenneth b
Just save the assembly as a part.
Reply to
Shemi Rubin
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.
--=20 Neville Williams (remove the "knot" to reply)
Reply to
Nev Williams

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