I am confused as to how to create and orient new reference planes starting from a base reference plane and not a part surface. For instance if I go to place a "coincident plane by axis" onto an existing reference plane it just drops the plane into the same orientation as the reference plane without allowing me to align the axis. Also, why when I create a coincident plane, won't Solid Edge allow me to use the n,b,t,f, and p keyboard shortcuts to orient the plane, like I can when selecting a part surface. I know there are workarounds, but this is highly annoying.
Yes, You have found an absolute fact.
Using any existing reference plane always will copy it as it is.
Any orientation only will work for faces AND coordinate systems!
My personal preference is to not use planes anymore if possible.
I prefer to use coordinate system.
The offer more flexibility especially in sync.
I work almost entirely in ordered so I don't know if sync can do this or not. I typically used "Angled" plane command to get the orientation I want and then I make a "Parallel" plane to that. Is there a reason why you want to use the "Coincident by Axis" command?
I have a part that I have created that is cylindrical in nature. I now have to emboss some text down the circumference with the text oriented so that the words run down the axis of the part, and it is easier if the plane is properly oriented to begin with. I have text oriented at various angles around the part, so I had to have various planes set up. I did this by creating a sketch like spokes on a wheel, and then using the plane perpendicular to curve command. That command does let me use the shortcut keys to orient the x asis. This really should be implemented for all plane creation methods, whether you are starting from a surface or a plane.
That sounds complicated. I am guessing you need a .par file. I have a method that may give you curved embossed letters. By the way this is a very round about approach.
1) Create a sheet metal part.
2) Put forms on the sheet metal with bends radius that are large enough to make the part a cylinder. (It will have to have a small opening but nearly a cylinder)
3) Unbend the part
4) Use the dimple command to put your text on the part. (I think you will have to use another dimple command for each letter)
5) Rebend the part
6) Save as .stp
7) Open the file as a .par
8) close the gap so that the part is a cylinder.
It really pretty easy. You just have to create planes outside the part. Then place your text in a sketch on those planes. Then use the project curve command to create a curve that maps down onto the part surface. Then you can use the extrude normal command and select the projected curves to make good letter extrusions.
I agree the it would be nice to be able to use n,b,t,f,p in all plane creation methods. I get this question every class.
I couldn'd resist mentioning that ordered features can be created on syncronous planes and sync planes can be manipulated easily.
Also, I am sure you know this but you can just create a line in the sketch at the angle you want before you create your text profile. The text profile will attach to the angled line.