3D sketch planes

So far I am real happy that Solidworks is taking 3D sketch up a notch. It is really fast and you can get a lot of design intent in one sketch.
I am finding that models rebuild more consistently and SWX doesnt seem to crash as often. But..problems will arise
I am having issues with the 3D skech planes when I apply horizontal relationships to spline endpoint control handles. Instead of the handles becoming horizontal to the world, the grid becomes parallel to the spline handle. In what world is that logical?
http://img382.imageshack.us/img382/9975/3dsketchsplineproblem7nh.gif
The workaround I have is to exit out of the 3D sketch plane by double clicking, and then create a horizontal line that I then have to go back into the spline sketch and make horizontal to. Blech!
Anyone figured out a better way?
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It's logical in the paradigm of each plane having a local coordinate system, similar to a 2d sketch, but very different from regular planes. This is a result of the plane being a sketch entity instead of a parent feature.
Reserve horizontal for those cases where you want to control orientation to the local sketch plane. Otherwise, look for options like "Along X" or make it parallel to your top plane. There are similar alternatives to the vertical relation.
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Dale, Thank you for explaining this to me. I dont fully understand the underlying logic of 3D sketch planes then. This is probably because I am thinking of the 3D sketch planes to be a more freeform version of the regular construction planes. Can you please post some explanation of how this localised coordinate system is used correctly?
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I'll try.
The new planes in 3DSketch are sketch entities, just like lines, arcs, splines, etc. Their positions and orientation solve along with all the other entities, including the entities on them. If you hold a piece of paper in space, the horizontal ruled lines on the paper can be in any orientation on the paper, with no regard to the world. If you rotate the paper, the lines are still horizontal to the paper, but may be vertical to the world. If you want the lines on the paper to be horizontal to the ground, you have to hold the paper that way. If the paper were a sketch plane in a 3DSketch, you could set the lines to be parallel to the ground, and then you wouldn't be able to rotate the paper anymore.
So, if I draw a rectangle on a sketch plane using the rectangle tool, the 4 lines will be added with horizontal and vertical relations. Those relations only have meaning within the sketch plane. To control the rectangle to the rest of the world, you need to make a relation between one of the lines in the rectangle and something ouside the sketch plane.
You may not be aware of it, but a 2d sketch on a reference plane (or a face) is not much different. By default, "horizontal" is aligned to the part or assembly coordinate system. This can be changed by a little known tool under tools, sketch tools, align, grid. Align grid will re-define horizontal in the sketch to be aligned with a model edge, instead of the global x axis.
As for how to use horizontal (and vertical) in a sketch plane in a 3DSketch, that's up to you, once you're aware that horizontal only has meaning within the sketh plane. You could create a construction line on the sketch plane, then apply some relation to that in order to control the orientation of the sketch plane. That might be most helpful to you, for the (probably) common case where you want horizontal to be aligned to the world, as it is by default in a 2d sketch. For all other cases, you can use horizontal and vertical within a sketch plane to quickly lay up geometry that will move together with the plane to whatever orientation you may need. For example, lofting between two rectangles, twisted 45 degrees from one another. Use the rectangle tool to draw the two rectangles, on two separante sketch planes. Make one of the lines in the first rectangle parallel to the world. In the second, apply an angle dimension to one of the lines to rotate it 45 degrees to the world. All the horizontal and vertical relations that define the second rectangle are now rotated 45 degrees because the plane has been rotated.
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Dale, Thank you for your clear reply. I wonder why Solidworks chose not to align the grid to the world by default. Thank you for telling me about the Align Grid command. This will be useful in larning new ways to sketch.
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Well, I'm glad it was clear. I wasn't sure it would be.
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