Get Datum to center of 2 surfaces
Get Datum to center of 2 surfaces
(OP)
Hi,
How do I get a datum to be at center or between 2 surfaces?
Thanks
How do I get a datum to be at center or between 2 surfaces?
Thanks
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Get Datum to center of 2 surfaces
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RE: Get Datum to center of 2 surfaces
FYI,
I'm trying to use this datum so I can create a section cut. Using WF 4.0 if someone needs to know.
RE: Get Datum to center of 2 surfaces
RE: Get Datum to center of 2 surfaces
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?
Thanks
RE: Get Datum to center of 2 surfaces
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.
Good luck.
RE: Get Datum to center of 2 surfaces
This makes 2 of us....
Capabilities between ProE & NX seem quite comparable, but the functionalities are quite different.
So, from what I see from the feedback here, ProE is not "smart" enough to distinguish two plan surfaces & find the center.
It appears that we have to do a manual measurement, then take that management & divide by 2.
A bit more work, but same result.....
Thanks
RE: Get Datum to center of 2 surfaces
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.
RE: Get Datum to center of 2 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.
Thanks Everyone....
RE: Get Datum to center of 2 surfaces
Joe Borg
RE: Get Datum to center of 2 surfaces
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.
Hope this helps,
Michael