probably dumb ? but...

[2ms1]

I need to horizantally and vertically center the joint/spring assembly against the face of the large segment shown below. I will be mating the two faces of course. And I can align the two vertical planes that run the centers of the two. But the best idea Ive come up with for centering them vertically is to add a datum plane to the large segment that is normal to the face, parallel to Top, and centered vertically. However, for some reason I cant think how to do this. Any suggestions? Im not so great at assembling things yet. Any better approaches would also be appreciated. Oh and while this picture is up...anyone know how to make the round on the big face facing out of picture only round the major edges rather than also rounding the inside of the little indent on bottom edge too?

View attachment 2367

View attachment 2368
2006-06-09_122828_1_2a.prt.zip
Edited by: 2ms1

 

[johral]

Prior to adding the rounds to the part, sketch an "X" (datum curve) using the four corners of the face as the references. Then you can put a datum point at the intersection. No matter what you do to the shape of the face, the center of the X will still be the center of the face (assuming it is symmetrical in one direction). You can then use the point as a reference for creating datum planes, axis, etc. to allow you to place the the other part during assembly.

 

[2ms1]

care to also tell me how to sketch an "x"? I only see CRV OPTIONS Thru Points, From File, Use Xsec, and From Equation for making datum curve. Ive never made datum curve before

 

[johral]

Insert/Model Datum/Sketch - pick the face where you want the point as your sketch plane and then sketch 2 diagonal lines from corner to corner (just like you would to create any gemoetry).

 

[ctolman]

You can use the curve option (through points) and select two corners to create each curve independently as well. This also allows you to do some cool things with creating tangencies for other models.


As far as the added round on the small surfacing goes, A round will always follow around any curved surface. Make sure to let the corner remain sharp until after you make the bigger round and Than add the smaller rounds you need later!

 

[superdutynick]

Point/Plane:
I would create a point on curve... pick the point tool, pick the edge, change the offset type to ratio (ratio is just as you would think from its name, real is the absolute value from the end), change the offset value to .5. The point will always be centered on that edge. You can then create your plane through that point.


Round:
After you select the round tool, select the first edge that you want to be round, hold down the shift key and click the same edge (notice the tangent chain disapears and just a single line is highlited), click the other edges to add to the chain while holding the shift key.

 

[2ms1]

superdutynick, thanks for the tip of points on edge with .5 ratio that
seems the most elegant for this particular application although I have
learned a lot of other things that will be very useful in future from
other posts on here

ctolman, please elaborate on what u mean by doing cool things with tangencies for other models.