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I have a feeling you would have better luck with something other than cavities. Anyway, what I would do would be to make a curve that represents the pattern, and then make a curve driven pattern of some sort of feature such as a revolved cut. If you have to do cavities, I recommend the Combine feature instead, and pattern bodies instead of features. Either way, you're in for some performance issues. I see you have a preference for non-ideal SolidWorks boxes.
If you are trying to make a 2 directional pattern on the part shown, I'm afraid you're SOL.
Is that a plastic or metal part? If its metal, will the pattern be applied in the flat? If so, maybe you could get away with applying a texture to the 3d part to make it look patterned. If its plastic and you have to mold it with dimples, well, good luck. 500 dimples will be very small or not leave much surface area left.
Anyway, best of luck.
I'm thinking face curves could be used to extract sketches that could define intersections where you could locate a series of sketch points in a 3D sketch. Then you could use that 3D sketch of the sketch points to drive patterning of the bodies as Matt mentioned. Creating 500 bodies and then performing an operation on them to deform or indent your target model is going to be very nasty performance wise.
Good luck! I tried this very same thing recently and gave up in SolidWorks, but then I don't have 8 cores of Mac power to go at it (guys really, 8 cores x 3GHz is about as good as it gets these days, and presumably backed up with a shed load of RAM? Patterning uses processor power not so much the graphics functionality I find - a pity then that SW modelling functions are not multi processor aware for most things).
A few (maybe helpful, maybe not) tips:
Do the pattern as a body pattern as Matt says then Combine ADD all the dimples/shapes into one, before subtracting. Don't ask me why but I've always found this works better on rebuilds.
Rather than worry about changing the pattern every time maybe consider using freeform features to change the underlying shape after patterning?
If doing that, consider exporting as Parasolid, importing as parasolid and working on a dumb shape - works quicker I find.
Patterning wise, I must admit I tend to do these kind of things with spheres to cut or add dimples to the surface/solid. Pattern by area works OK, but many times I end up placing points then manually placing the dimples on those points. Not ideal but it does work.
Last resort - export to another package that does this better than SW - I tend to use VX for this stuff, but I have seen an associate with Pro/E in action on patterning at it has a lot more options.
Edit of above - SolidWorks could do with beefing up its patterning on surface tools - this kind of task is commonplace for grips and the like. VX does it like this:
That was 4 versions ago....
Further edit. That tool in VX is OK but not idea. What is needed in SW is a tool where you can define a body as the tool to cut the dimple or a feature to add relief, then select surface faces and pattern based on visual parameters rather than values (which always go astray on curvy forms). By visual I mean, select the surfaces in the original example above to add/remove dimples to, select the body to remove or a library feature to add, then simply have a slider to vary the visual density of the pattern.
This way when the part is reshaped the visual density is constant and the pattern adjusts accordingly.
The clever part of course is what happens at the edges. Maybe in these cases selecting the faces creates an overall border for the pattern surfaces and the density parameter can be faded out across a user defined zone?
That tool alone would be worth every penny of the subs for me.
That VX stuff looks like what I need, but then Rhino claims to do the same ( http://www.rhino3d.com/features.htm), but surfaces out of Rhino is mostly problem.
I'll have a look at VX when I get a chance.
And yes, these parts IS nasty performance wise. SW need to have a look at the multiprocessor support. But SP2.0 was a pleasant surprise, some well aimed work done on Photoworks!
The patterned part is a molded elastomer (it is a grip-surface on a pilot-style handle), so I guess the mold will handle the cavities. But I have no experiences from molding elastic materials, so this might be interesting in more than one way
Design is the mayor selling-point, so I don't think they ever give this up just because I don't have enough hardware/software backup (jepp, new Mac Pro now has 8 x 3,2Ghz and 1.6Ghz FSB so I no longer can tell them I have the fastest computer around and that it cant be done that was a convenient trick though).
Points on the surfaces and then mating balls in these, and then cutting with them, that is amongst what I have tried.
But since the time-budget is tuff on this one I don't find a rational way to make the pattern flow nicely using that method.
First I made construction-lines between the points, and had the points mated "on surface", but that don't makes a pretty pattern, and time flies while doing these.
Spline on surface is very "nervous" feature in SW, and specially while the splines cross multiple surfaces and more that 180° change in the surface normal direction. That would have helped me to fix the flow though, but also a huge amount of time.
I think I'll try tomorrow to use Rhino to make geometry that I import and mate in 3D-sketch-axes to, and then mate my cut-spheres to these. I'll combine these to one body as suggested, thanks for helping.