C'Bore hole in round part

[Steve34208]

I am new to SW and having a very difficult time placing a 1/4 c'bore in a round part off center. The round part has a hole thru the middle used to clamp on a shaft. There is a counter bore then tapped hole off center to allow the clamping function. I know this is probably very simple, but I can't figure it out.
Thanks,
Steve

 

[DesignSmith]

Here is the trick.
1. Insert - Reference Geometry - Plane - {On Surface}
a. and click anywhere on the cylinder OD
2. With that new plane still active, click the Hole Wizard command button.
a. type over the C'Bore depth values in the dialog, to force your hole to intersect the cylinder properly.
b. it will be easier to dimension the hole location point, if you cylinder was symetric about the part origin.

If you don't start the Hole Wizard command by pre-selecting a flat face, the location point is a 3D sketch point and can be moved around accordingly. By using the reference plane you force the start point of the hole to be on a tanget to the cylinder but you can still dimension it to be off-center.

FYI,

DesignSmith

http://www.DesignSmith-Services.com

 

[Steve34208]

Thanks DesignSmith,
That works great.

 

[Regg]

Steve34208,

If you have a sawcut to split your collar, you can also select the flat surface created by the it. You then "flip" the entries for the counterbore diameter and hole diameter. Since, where I work, we dimension the counterbore depth from this flat anyway, the counterbore depth becomes this dimension so it can be inserted into the drawing.

Regg

 

[Steve34208]

Thanks Regg,
I do have a saw cut but I was trying to flip the counter bore. I didn't think of flipping the entries. I like that solution.