Adding threaded holes to a nearly completed part?

[luke1201]

I've got a small part that I'm almost done with. All that is left is to add 4 small threaded bolt holes (4-48). The problem is that I can't seem to position/locate these holes exactly. What I want to do is create points for the center of each bolt hole, smart dimension them to the exact position I want, then use the hole wizard and use those points.

I can create the points, but when I try to use smart dimension, to move them into the exact position I want, it tells me the drawing is over-defined. Or it will only make a driven dimension and I can't edit it to move the point.

I've also tried a similar method of creating lines (temporary) to create intersections where I will point the hole wizard, but have the same results, either I can't edit the dimensions or its over defined.

How can I fix this?

 

[Heckdogg]

Why not just create the holes with the hole wizard, then edit the hole wizard sketch to add the dimensions to the hole wizard points to locate the tapped holes where you want them?

SolidWorks 2005 SP01.1
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[MElam]

Heckdogg is right. Adding the points in the Hole Wizard feature does the exact same thing without a duplicate sketch.

One thing to watch - be sure to pick the face you want to place the holes on before activating the hole wizard feature. This will ensure you are working in a 2D sketch instead of a 3D sketch (and is much easier to work with as far as positioning).

Something to check in your existing sketch - select the points that are going over-defined and see if you have inadvertently picked up a relation to another object (most likely a coincident)

 

[drawoh]

luke1201,

You can draw lines when sketching in the hole wizard. I do this all the time, since it simplifies dimensioning, and makes the intended geometry a lot clearer.

JHG

 

[ctopher]

The others are correct. In the feature tree, under the hole wizard, there are two sketches. Edit the 3DSketch and position/dimension the points (center of holes). You can copy them also in the same sketch to make more holes.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
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[luke1201]

Thanks guys, thats what I was missing, editing the sketch created by hole wizard. That did the trick.