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Problem with sketch reference orientation

That is not an approach I have ever used, if you can show a picture there may be an easier way. However, to answer your questions:

The horizontal or vertical reference datums need to be normal to the sketching plane. You may need to add some additional datums just for these references. Make the reference datum through two of the points and normal to the sketching datum. You can also use edges instead of datums which might be better for you.

The smallest (thinnest) dimension in Pro/E is determined by the part accuracy and the size of the part. If you use the default relative accuracy of .0012 the the smallest dimension is .0012 times the length of the diagonal of a box containing the part. You can find the length of the bounding box diagonal by picking INFO / MODEL SIZE. You can change the value of the accuracy or change it from relative to absolute by picking EDIT / SETUP / ACCURACY.

If you have really thin features you may want to create surfaces rather than solid features. You can always thicken the surfaces later.
 
How can i solve my problem...
I cant make datumplane as a refence to normal datum, because i need all three datums referencepoints to define the parts surface.

Is there somekind of other way to define that surfaces three referencepoints? As a groupreference that could be used in that kind of situation?

And here is the part...
http://mathworld.wolfram.com/SzilassiPolyhedron.html






Edited by: Vezku-
 
Vezku- said:
How can i solve my problem...
I cant make datumplane as a refence to normal datum, because i need all three datums referencepoints to define the parts surface.
Of course you can. Make the sketching plane thru 3 points. Then make the horizontal or vertical reference plane thru 2 of the same 3 points and normal to the sketching plane you just made. I have attached a very simple file with just a csys, 3 points and one solid feature made with the sketching plane and reference plane made on the fly referencing just the 3 points.
2006-03-31_095249_3pointprt.zip
 
Thanks, now it works... but i ran into new problem. How i can use more than three referencepoint for sketchdatum?
Some of the sides are so complex, that three referencepoint isn
 
Well, three points always define a plane (if they are not colinear), anymore and it would be either overconstrained or invalid. You can create all the datum points, axis or curves you might want on the sketch plane.
 
Vesku


Create a point feature. you can specify more that one point offset from a coordinate system. Can you post your part? It seems to me you are having a tough time with it, we may be able to help better if we have a look at it.


Sip
 
Getting better!

I noticed that i had given wrong value no Z-coordinate at N-point. (stupid me
smiley9.gif
)
Fixed that and part became ready. Still one question. How i can apply different colors to different sides when they are defined only as a surface? Or is this possible at all?

Thank you all! This is a great forum!
 

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