I've been trying to add reference planes to a sheet metal part by rolling back to before the first sheet metal feature (I want to place the SM sketches on new planes)
but when I try to put the sketches on the new planes they are greyed out, like wise if I want to add and use a new sketch to use in the SM base feature,
how can I get these to be includable
SW2010 SP5
Known bug - SPR# 583949
Thought it was mis-behaving, as I could do the same thing with a normal part ok, but not in sheetmetal, has this been fixed since 2010?
Not yet.
Which OS has this problem? I'm running XP x32 and have never had, or heard of, that problem.
I can repro in Win7 x64. I'll try XP too and let you know.
Yep Win7 x64 here to
This sounds a bit strange to me as well. I just tried a test and it worked fine. Maybe give this a try to see what you get.
I created a test sheet metal part by clicking on the front plane, putting a rectangle sketch there and creating the base flange. Then I Ctrl-dragged the front plane to create a new plane, which placed that plane at the bottom of the tree. Then I drug that plane up to the top right under the origin and before the Sheet-Metal1 feature. Then LMB on the base flange sketch and Edit Sketch Plane and pick the new one. All worked fine.
Notice that I didn't use the rollback bar. When I tried basically the same thing by pulling up the rollback bar & creating the plane, I was then not able to select that plane for the sketch.
I basically always use the first method so that's why I had not seen this one before.
WT
Wayne, with your second workflow you just reproduced the problem listed in that SPR. Good to know that there is a simple workaround.
Yup! :-)
WT
I automatically used the same method as Wayne because there was no need to use the Rollback Bar; But after using the Rollback Bar I see the problem.
However, the planes (created using the Rollback Bar) become selectable if they are relocated (by dragging) in the Feature Manager ... even if they are returned to the same location.
Kelvin, thanks for the workaround! Nice find.
Thanks for you help guys, these workarounds will do me fine..
Thanks Kelvin Lamport 
This sounds a bit strange to me as well. I just tried a test and it worked fine. Maybe give this a try to see what you get.
I created a test sheet metal part by clicking on the front plane, putting a rectangle sketch there and creating the base flange. Then I Ctrl-dragged the front plane to create a new plane, which placed that plane at the bottom of the tree. Then I drug that plane up to the top right under the origin and before the Sheet-Metal1 feature. Then LMB on the base flange sketch and Edit Sketch Plane and pick the new one. All worked fine.
Notice that I didn't use the rollback bar. When I tried basically the same thing by pulling up the rollback bar & creating the plane, I was then not able to select that plane for the sketch.
I basically always use the first method so that's why I had not seen this one before.
WT