I created a layout sketch on the X-Y plane by accident, now I want that sketch to appear in the X-Z plane. Is there an easy way to switch this?
You can Right mouse click on your sketch and it will let you edit the sketch plane.
Then click the face or plane you wish to use.
DJ, I'm assuming you're talking specifically about the assembly layout sketch functionality and not just an ordinary sketch.
the assembly layout sketch is actually a 3D sketch. If you happen to have a plane selected when you launch it, the layout engine will effectively do a '3DSketch on plane' operation to constrain the sketch entities you create to that plane. You can exit this mode by right-clicking (while editing in the layout sketch) over an empty area of your screen and selecting '3D Sketch on Plane' again.
Select a flat face or plane, rmb and do 3D Sketch on plane again to change planes.
OK, onto your question. If you have already drawn in the layout sketch geometry on the XY plane, probably the best way to change the plane of the sketch is:
The advantage of this approach is that it preserves the relative orientation of the sketch geometry.
Hope that helps.
That's what I was looking for, except I can't seem to make a block from the layout sketch. Everything seems to be selected, but when I click OK nothing happens - I should be able to insert that block again but no blocks are available for selection. I have already inserted parts into the layout that I currently have suppressed, maybe that is what's stopping me?
Since John hasn't answered, I will give it a try. Unfortunately, I hardly ever use blocks or 3D Sketches and I never use Layout Sketches, so I'm not too likely to be of much help. It seems likely that John's method would work, so I wonder if you might have some elements in your 3D Sketch that aren't in the XY plane. I could imagine that might stop SolidWorks from making a block out of your entities.
DJ, it looks like the geometry has to be planar in order to make a block out of it.
try selecting your geometry going to tools==>Sketch tools==>Rotate
uncheck the 'keep relations' control and drag the appropriate hoop on the gizmo to rotate the geometry
This will remove any relations between the selected geometry and the rest of the layout and assembly. Relations between entitites in the selection will be preserved.
I'm using SW2012. The "Create Layout" command defaults to start the 3D sketch on the front plane, but I would like it to start on the Top plane. Is there any way to change the default behavior to begin the sketch on the Top plane?
If I start the sketch on the default front plane, and then sketch a few simple shapes on that sketch, and convert each shape into a block, and then convert each block into a part, the front plane of each part correspods with the front plane of the layout sketch. That's consistent behaviour.
But if I start the 3D layout sketch on the Top Plane, and sketch the same simple shapes on that sketch, convert them to blocks, and convert each block into a part, then the Front plane of each part is mated with the Top Plane of my layout sketch. Thats cuckoo; I want the top plane of each part to be mated with the top plane of the layout sketch.
Why does SW have to make this so difficult?
I came here with a similar question. I just wanted to create a layout sketch on a different plane, but this will also solve the problem of transferring which plane your sketch is on in a much easier fashion.
1. You select which plane to start your layout on.
2. Draw your layout.
3. Oh no its on the wrong plane and I don't want to start over!
4. Select all the entities in your layout sketch.
5. Ctrl+C (copy entities to the clipboard)
6. Right click outside the sketch to create a new plane to sketch on in your 3D layout sketch. Now you have multiple planes in your 3d layout sketch.
7. Ctrl+V (paste entities onto new plane). I find this easier than making blocks and/or remaking sketches.
As for 3D layout sketches, you can make them, but it seems only by deleting the on plane relation that is automatically created with each sketch entity. I don't see how layout sketches are any more useful than a regular sketch in the assembly. Maybe someone else could explain that.
Bonus Tip: I'm drawing a layout sketch on top of some components that are already in my assembly, but I couldn't create relations to them. Because the layout sketches are default in plane, you can't create relations to edges that are not in your layout plane. Use the "On Plane" relation to mate your entities to the face that coincides with the edge you were trying to mate to.
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