Are you creating a point pattern of the same hole at the part level?
I created a sketch using lines so I could project them onto multiple surfaces. I created a single datum point feature with multiple points using the vertices of the projected sketch. I created an axis at the 1st instance hole so I could select the surface and axis for placement. I then used the point pattern. You need to understand this tip, however, select the origin! Use the point at the 1st instance to create the origin. I suggest you do this prior to selecting the point location feature because the black dots get in the way of selection.
The tip is something PTC really needs to look at. The 1st instance assumes a "feature center" as the starting point while placement according to the points is at the surface. This causes an offset of all the features including duplicating the 1st instance! The fact that you cannot select anything under the dots is a secondary issue that this interface really doesn't address. So setting the origin -before- selecting the point set is yet another Pro|WorkAround^tm to deal with this critical but little understood assumption by PTC. In this case, it is obvious, but there are all too many occasions when this offset is minute and perpetuates a significant error.
Correct pattern with selected origin:
Default assumed origin
Hi, and thanks for a quick reply 
I started a sketch at the top surface, then added point datums, added dimensions, do all datums are on the same level. I get this message:
This feature is defined with dimensions that are very small compared to the rest of the part.
You may want to change the part accuracy to be smaller than 7.72427e-05.
I have set the accuracy to Relative 0.0001, but it still failt.
I'm still new to Creo, but I will try your metheod now (just need to read it closely to understand it).
But thanks for the help so far.
Holding the Ctrl key is normally how you get multiple selections. You can also open the Details dialog to aid in selection.
Still failt here, not sure why. I can make single independent hole, but not when I chose axis and surface.
I added the axis on the point, and used the surface as a reference. I will test axis as a assembly feature, as soon as I get to work tommorow 16 hours is enough for 1 day
But the weird thing is that it worked with extrude for me, but not hole. But I guess PTC Creo works in mysterious ways...sometimes...
I appreciate the help you have given me so far
I gave this option a try in assembly mode.
I created a sketch on each part at the assembly level using various references; both part and assembly. Sketch 1, 2 and 3 have geometry points fully defined.
Axis AA_1 was created from a point and surface reference.
And a common group of points was generated (datum point id 46) by picking all the sketched point. We don't have assembly datum intent features (only in part mode) so I had to recreate the set to put them in a single feature for point pattern selection.
Since each projection in our earlier conversation had to be a separate feature anyway, why not just create the sketch on the appropriate plane. Even if you have an over-reaching master sketch, you can use these references for the individual sketches for placing geometry points.
Please understand the difference in sketch mode between construction points and geometry point. Geometry points will create a datum point that remains selectable where a construction point does not once the sketch is closed. The Geometry point is created at the Datum tab where the construction point is in the Sketching tab. This is true of axes and coordinate systems as well.
Again, I had to pick the alternate origin in creating the pattern, but it is working very consistently when selecting the point feature in the assembly tree. Remember to show Features in the tree options.
Attached is the assembly in Creo 2.0 full version. Feel free to interrogate the model to see why this one is different from yours.
