Use datum plane tool and place it wherever you want with offset translation, name it as you want, then, when you make Xsec use that plane as a reference for it.
From the description you just gave me, it does not appear that ProE is smart enough to find the center of 2 surface areas. It appears that I need to measure or determine the center myself, if I want to place a datum in the center.
I hope I am wrong with this high-power CAD application. Perhaps, I'm comparing to NX because I'm more familiar with NX, but I would think this would be a normal function within ProE in any version.
Can anyone anyone answer or suggest another alternative or is this the only way to do this?
Oh man, I spent a while the other day trying to figure this out. Pro/E is really making me miss NX.
The only way I found to do a bisector between two planes is figure out where I defined the two planes, luckily for me it was a single cut extrude. I then created a relation to call that dimension and divided it by two.
You could place the plane where you want it and then extrude the feature creating the surfaces in both directions. That way the datum drives the surfaces and always stays centered.
If you have to create the datum later & want it to automatically center as the surfaces move, you can create an analysis feature first & then use the result in an equation to drive the offset plane. This kind of thing is far more powerful than a built in mid-plane feature that only works for a tiny subset of potential geometry, namely parallel flat surfaces.
Interesting suggestion to tie the analysis to an equation. I'll have to check this out.
This question is for anyone:
If I want to link or associate one dimension to another, how do I do this?
In this particular instance, I have a sketch feature that was offset from center at a specified distance. Perhaps, similar to what's suggested above, I link or associate my new datum, plus add an additional offset.
I'm just not familiar on how to associate one dim to another.
You can use relations in proe. Go tools, relations. I suggest you find some tutorials or a good book on this. Relations can be quite messy. Each dimension has its own unique symbolic name. If it is a feature dimension is is a numbe prefixed by d. If it is sketcher dimensions it is a number prefixed by sd.
Probably the Easiest Way to do this is to create a datum point midpoint at .5 ratio along edge between your 2 surfaces then do a Plane through Point normal to edge or parallel to one of the 2 surfaces you want the midplane for.
Then you won't need to enter a relation.
Relation for an offset plane can be entered by typing the dimension symbol "d##/2" when modifying the dimension in the Modify Value field such as "d39/2", Pro/E will then ask you if you want to add a relation d52 = d39/2 and you can hit Yes . I believe the dimension symbol is shown in the help text when hovering over a dimension otherwise you can select Info>Switch Dimensions from the pull-down menus.
I remember NX having problems with Parametric points of this type till NX2 It seemed the .5 worked during creation but then it was just a non parametric x,y,z value. SolidWorks 2010 has a nice midplane Feature where you select two faces and instantly get a midplane like you've described above.
If you are talking about a trapezoid shape where you want a bisector midplane you can do so with 2 midpoint relations in a sketch.
Are the 2 faces planar? I believe NX also had a Midsurface option for non planar surfaces.
I myself missed NX2's sketcher selection based constraint toolbar until WF5.
