component pattern

I've patterned a component in an assembly... its a pin that can slide
up and down a hole. When I move 1 pin all the others that are patterned
from that pin move as well. Is there any way to delete their relations
so that I can slide each pin individually, but still using this pattern
method (as I dont want to have to mate 500 pins to 500 holes
individually)?

 

Sounds like you want your cake and eat it too. Think about the logic of
what you are saying. The idea of a pattern is that you have one part
controlling others. Now you want to have that one part control all the
others, but not in all directions. I understand your request, but can't
think of any way to do it.

Or, is it maybe just the first pin you would want to move without all the
others moving? If so, put it in by itself, and then put in the next one to
use as the pattern seed.

WT

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'Sounds like you want your cake and eat it too'

thats when you know you really are using some good software!. Its nice
when software just seems to work. Unfirtunately you dont very often get
that feeling with Solidworks.

 

Try the Right Mouse Button click & choose "dissolve pattern" Then you will
have 500 individually placed pins (not mated but they will be in the correct
positions)... unfortunately if you need all of them to stay cylindrical to
the holes but all move individually you will have to manually mate them in.

If that is the case it sounds like you should be using smart mates -- mate
one pin in the hole & the hold down the CTRL key while dragging the
cylindrical face of the pin & drop it on the next cylindrical face of the
next hole. This will copy the first pin & make a cylindrical mate to the
next hole all in one motion. Do that 500 times & now you got 500 pins that
all move up & down. if you look in the help file it will show you have to
predefine that face in a "mate reference" that way you don't have to drop
from face to face you can just drop it on the hole.

Have fun -- hope that makes it at least easier
Steve T.

 

ok thanks, I'll try that. Any ideas on how to mate two oval surfaces?
Image the pins are an extrude from an oval and the holes a cut from an
oval. I cant seem to mate them.

 

You can have your cake and eat it too.

1. Make two configs of a subassembly with just the pin.
2. Use planes to mate the subassembly.
3. Mate and pattern.
4. Make the movable pin a different config from the rest and set to
flexible assembly.

If this works you should be able to move one pin in the pattern.

 

Hmmm, interesting thought. Sometimes flexible subs cause issues, but worth
a try. Interesting indeed.

WT

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I made a sub assembly of the 2 pins (there are both mated in the same
position so that it appears as if you can just see one pin). I then
mated this sub assembly to the hole and patterned it. Of that sub
assembly I made 2 different configurations. I then set one to flexible
but when I move a pin the mates from the original are lost and the pin
is no longer mated to the hole... it is flexible in any direction.

Not sure if i've done this correctly though!

 

You'll probably have to use planes and/or sketch geometry to do your mates.
I would make my pins centered on the Front and Right planes. A sketch point
at the center of the holes can be used for the centering, with parallel or
perpendicular planes giving the alignment.

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

 

Pins from an oval ought to be able to have a axis.

Oval Holes could have an axis at their center.

Aligning the axes is easy.

Bo

 

Depending on how your ovals were created, you may still be able to use
conventional mates. If the ovals were made from 4 tangent arc segments,
concentric would still work, but would need to be used twice for each pin.
Even if the ovals are made from an ellipse, you can probably find tangent
arcs that create the same shape ( within a very small margin ).