Others have asked this question before. I used the hole wizard to create a hole and then used the curve-driven pattern. It created the pattern but some of the holes in the pattern are facing in the opposite direction, therefore they are not extruding the surface. How can I solve this? Also is there a way I can get the holes to be curved circular indents rather than straight holes? I've attached an image of the look I'm going for.
Sound like you are after spherical indents like in a golf ball?
If so, you can make the correct sized sphere, offset if from the surface this distance you need, pattern to where you want then Boolean remove.
You could then fillet the edges with a surface fillet.
I suspect the number of holes you are dealing with will take a bit of time to process. So, you do it, get it all working then suppress the features until the model is completed.
I use ZW3D but expect you can do this in SWx no problem.
The problem is caused by your drive curve. Make a plane parallel to your front plane through the point used to drill your hole. Rollback to before you drilled the hole, offset the 2 outside faces to surfaces at 0 offset (ie. copy them). Roll to end, insert new sketch on the plane you created. Perform intersection curve, sketch now has 2 splines, select splines and convert to spline - set tolerance pretty tight. Now perform curve driven pattern, using your new single spline as the driving geometry and select 'tangent to curve' They should all align the way you want. However because of the nature of these surfaces you are better off to pattern a separate body that can extend beyond the outside face of your part, then boolean subtract. But what you are doing will work.
I have come across similar problems myself- putting a hole on a curved surface (I don't know too much about Solidworks but have many experience with Inventor and AutoCAD). With Inventor the best way to do this is to make a work plane where you want the hole using the " plane tangent to surface through point" or "tangent to surface parallel to plane" feature. Then once you have your work plane in place use the hole command. If you want to make a bunch of holes (like in a golf ball) then make one and use the pattern command to make the rest.