cam mate

I am having problems with mating. Please take a look at
http://i226.photobucket.com/albums/dd113/sethr_bucket/sp0410ba1.jpg
(make sure you click the "full size" button in the upper left)

Basically, it is 2 cylindrical shafts telescoped together, with a
dowel pin in one, and a pin slot for the pin to follow in the other.

I can not get a cam mate to work at all. I have even tried creating a
surface body to "complete" the pin slot, but that doesn't work either.

I have tried alternate methods to mate this by trying to create a
projected curve on either the centerline of the slot or the profile of
the slot, and using surfaces, faces, sketch entities, etc. on the pin
to mate with. But SW will not allow me to even select the curve, even
though the help file says that you can do a curve to point coincident
mate.

I have tried everything else that I know of, both conventional and not
so conventional, but have had no luck.....

Anyone want to take a stab at this one? I would greatly appreciate
it.... Might even buy ya a drink in San Diego in a few weeks if you
are there....

Thanks,
Seth

 

I can't get to your jpg, but as a thought, can you set an axis of the pin to
a distance mate from either end of the slot? Maybe have to add planes, etc,
but possibility?

WT

 

Wayne,

Nice thought considering you can't see the picture. But the slot is
not a simple straight slot. Imagine a straight slot along the axis
direction, with a 90° turn at each end to "lock" the inside cylinder
from moving along the axis, on both ends.

One of the tricky things is that one of the ends that has the 90° turn
is "open" on the far side. It's kinda hard to explain. That's why I
posted the picture. But, I thought I would compensate for this
problem by adding a closed surface body to complete the slot loop.
But that didn't work either.

By the way, why couldn't you see the picture? Bad link? Firewall?
Etc.? I am asking to see if I posted the link correctly. If I did it
wrong, then nobody would be able to see it. That wouldn't be very
worthwhile... I would need to repost the picture link somehow.

Seth

 

By the way, why couldn't you see the picture?  Bad link? Firewall?

Seth,

I was able to see it when I clicked on the link. My computer opened it
in IE. Sorry, but I don't have time to mess with it right now. Work
has me covered up, but that's a good thing.

Reaper.

 

I love stumping the noncertifiedsolidworksguru.

 

I couldn't see the pic because of our SonicWALL filter here. It has that
site tagged as pornography. Maybe your mating then is related??

You could send me the pic directly.

WT

 

That was a good one...
You should have the pic in your personal email.

Seth

 

I've done this type of mate before. Cam Mate can't do it because it
requires the cam faces to be straight in one direction, as if they were
extruded.

You're on the right track with an offset surface but it gets complicated
fast. The basic problem is that you can't mate coincident to to more than
one face. So, what you need to do is approximate the cam path with a
single fitted spline. Since that only works in a 2D sketch, you then need
to use a wrap or a sheet metal bend on a temporary body to create a
surface from the fitted spline. This surface should have only one face.
Then you can mate the point from the pin hole to this new surface.

Sometimes, the surface gets wavy, or gets broken into multiple faces. Try
fiddling with the fit tolerance on the spline.

Even with this working, dragging the outer tube may be flaky. Sometimes
moving the part with a Spaceball works better than dragging with the
mouse, sometimes not. Some days it work as smoothly as you would hope.
You also get a built in limit mate, since the fitted-spline surface is a
procedural surface: the mated point won't go past the end of the surface.

You mention mating to the curve, which I've never tried. That should
work, but you may get overdefined mate problems with the concentricity of
the cylinders. I seem to remember reading somewhere thet curves can only
be selected from the FMT. I don'tknow why they won't let you select them
in the graphics area. Maybe this information is out of date. I just tried
a couple curve entities in 07 SP5.0, and I was able to select them. I
should try the curve method someday.

I hope that at least gets you to a viable idea.

 

Debbie,

I knew that was a cam mate rule. So, I tried creating a surface body
that "closed" the end that is open, and use this surface body to mate
to. Couldn't get that one to work either.

Seth

 

How about a surface on the centerline of the slot (or the closed up slot on
the end) to an axis on the pin? If it works I'll take a beer in SD.

Jerry Steiger

 

This sounds like there may be a solution buried in there
somewhere ;-)... Thanks. I'll play with these ideas.

As for selecting a curve, I could ONLY select the curve graphics
area. And only then, could only select part of the curve (which I
didn't even think was possible)....

Seth

 

This sounds like there may be a solution buried in there

I think I have something I could send as an example, if you need it.

 

Yes please! This is just about to drive me crazy.... I'm about ready
to cave and send it to my VAR.... The only reason I haven't so far
is, I want to finish this today, not a week from now....

Please send to
get rid of the NOSPAM of course.

Thanks,
Seth

 

Tried that. I have not been able to get that to work either... But I
guess I could buy you a beer for the attempt anyway.... ;-)

Seth

 

I hope SW07 files are OK. On their way...

 

Just for a try, convert the faces of the slot to one single surface.
Then sketch a point on the surface of the dowel and give a coincident
mate to the surface and point.


Deepak

 

I tried that early on. The problem there is that you can convert the
slot faces to one surface body as you mention, but it will still
contain multiple faces. You can only mate a point coincident with one
face.

I did end up doing something very similar as well.... I found a way
to get the mate to "track" correctly. I simply extruded a fitspline
surface (one face) along the centerline of the slot, created a sketch
point on the dowel axis in a position that it contacts the surface in
the slot.

It moves really well. The only problem now it that it doesn't "stop"
at the ends of the slot. I tried using an angle limit mate to confine
the rotation to stop at a desired angle. But as you might expect,
every variation that I tried either over-defined it, or caused it to
"jump" past where it should for some reason....

I think I will give up now....

 

"I did end up doing something very similar as well.... I found a way
to get the mate to "track" correctly. I simply extruded a fitspline
surface (one face) along the centerline of the slot, created a sketch
point on the dowel axis in a position that it contacts the surface in
the slot.

"It moves really well. The only problem now it that it doesn't "stop"
at the ends of the slot."

This seems strange. Since the path is a spline, how does it extend it?
Somehow it "knows" that the ends are really straight lines? Try putting a
fairly sharp kink at the ends of your spline. That might stop SW from
extending the spline. If it doesn't, at least you get a signal that you've
reached the end of the "real" slot.

Jerry Steiger

 

I did not have time to post last night to show something but you
concluded the same... here are my layout files for all...

http://www.zxys.com/misc/teleslot-zxys.avi
http://www.zxys.com/misc/teleslot-zxys.zip

... (if SW Corp only used their program, maybe there would not be as
many problems..?)