How to copy a point onto another plane while aligning with the original point?

Hi,

I have an extruded surface with a point on it and would like to copy
this point to the opposite side of the surface (parallel plane) while
keeping it in the same spot that it would be at if the planes were on
top of each other. The best way I've found to do this so far is to
smart dimension both points but I would prefer a method that will move
both points if one point moved.

Also, when I am looking at the opposite side of the extrusion, is there
a way to stop points and lines on the former side from showing through
(other than hiding individual sketches)? I've tried adjusting
transparency and switching to opaque but this seemed to have no effect.


I've noticed that if I extrude a rectangle and there was anything else
sketched (inside or outside the rectangle), these parts of the sketch
disappear after the extrusion. I'm guessing this is because of the
hierarchy used by the property manager but if there is a way to display
the entire sketch I'd like to know how.

I'm putting points on both sides of extrusions in an attempt to line up
electronic panel-mount components (I'm making a top and bottom as two
separate parts) with the panel (surface) they are to be mounted to. If
anyone has a recommendation on a better method to use I'd love to read
it. I've been considering cutting a hole in the surface and trying to
line the components up with that but I'm worried this will make it more
difficult to move the components. I'd still like to have an answer to
the original questions, even if a better method is mentioned.

Thanks much,

David.

 

You could insert your second point. Make it Coincident with the first
point. Then delete that Coincident relation. That would get the second
point to the same location, yet be unconstrained.

Ken

 

If I understand you correctly, could you just use "convert entities"
sketch tool? This would project the first point onto your second plane
(which is parallel) and keep an updated location.
I'm not sure about the sketch view. You can turn off all sketches in
the View menu, but that may not be what you want.
~Alex

 

But how could I insert it onto a different plane? When I try to move a
point in a sketch I am unable to move off of the current sketch plane
and when I make a new sketch I am unable to add a relation between the
two... Plus coincident would require them to be on the same plane,
correct?

Dave

 

No, you can make a coincident mate to sketch entities on different
planes, but keep in mind they are projected to the active plane. So,
if the planes are parallel, you can simply use the "convert entities"
tool which projects the selected objects (lines, points, arcs, model
edges, etc" into the current sketch with "on edge" mates which are
parametric (will update to original geometry).

make a new sketch on the plane you want, and select "convert entities"
and you're done.
You could also just sketch a point, and then select that point and the
point you want to mate to "ctrl select" and hit the coincident mate.
Either one will work, the convert entities tool does it all in one
shot.

Rather than thinking of moving the point off the current sketch to
another, think of it more like creating a new point in a different
plane and having them "overlay". I do this all the time and it works
great.

It's another big difference between SW and the way AutoCAD or other
static cad programs work.

 

When you create a feature, such as your extrusion, SolidWorks automatically
hides the sketch, or sketches for features like lofts and sweeps that use
more than one. You just need to expose the sketch (left mouse button on the
+ to the right of the feature), select the sketch (right mouse button) and
"Show" it. (I think that's right. SolidWorks is in the middle of a long
rebuild and I can't check it.)

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

 

I'm surely no expert with SW, but this seems to be pretty basic to the whole
gestalt of assembly modeling. "Convert entities" projects geometry onto the
sketch (for your cut outs, for example). Unselecting "No External
References" (the default) in the assembly maintains the relationships to the
reference part. The cutout and hole features follow your object when you
move things around.