Another reference pattern problem

Hi John...

You've been bitten by the dreaded rotational pattern bug. The problem is the way you specified the cosmetic sketch. You chose two axes and aligned your sketch to them. You'd expect that this would pattern correctly, and it DOES, until you passed the 180 degree mark. Suddenly, your pattern starts misbehaving. This is common.

Whenever you have a pattern that stops working passed the 180 degree mark, you've got to change the way the features within that pattern are being defined.

I see why you're using the pattern table and I understand what you're going for. I would have approached this problem differently. Back in the old days, when you wanted something to rotate in a pattern, you gave it an angle and varied the angle dimension. Or, you made a datum through an axes at some angle... tied your feature to it... and then varied the angle dimension. This caused routine problems when your pattern rotated beyond 180 degrees. Your pattern would stop working... or, if you used the datum plane method, the datum plane would "flip" at 180 degrees. It was maddening. You ended up making all sorts of features to try to force the pattern to "stick" where you wanted it.

Then, finally PTC gave us the rotational pattern (pattern around an axis). Suddenly, the skies cleared, the oceans began to recede, and the Earth began to heal... oh wait, wrong topic!

The point is... the rotational/axis pattern solved most of the problems with misbehaving geometry. In your case, you've tried to use table pattern (which was another popular method to avoid the pattern problems). While I commend your use of this feature, it probably contributed to the cosmetic problem.

I've attached two files:

• johns_part_old_pattern - uses your original table pattern and solves the problem by creating an on-the-fly datum plane during the setup of the cosmetic sketch. This stops the pattern from failing and creates the desired geometry and the cosmetic sketch.
• johns_part_new_pattern - this is the way I would have done it. I used a rotational pattern spaced evenly. I think I just evenly spaced 8 holes (which would be 45 degree offsets) but I turned off the two pattern members along the parting line (the center ones) so we were left with the desired 6 hole pattern. I kept the grouping similar to yours but you'll notice I have less features (therefore less to fail).

You can make a good case for several other approaches, too. Unless I'm doing something crazy, I don't bother with the hassle of table patterns anymore. They're still very powerful but with a few notation exceptions I go with one of the newer, simplier approaches. I'm not a proponent of simplification at all costs... I try to simplify when I can but still use the powerful features when they're needed.

There's one other tweak added to the new file... I changed the pattern options so the driving pattern (first one) is set to Indentical. For a part this small, you won't notice much of a difference but if this part will have multiple holes, changing your patterns to identical can pay off big in decreased regeneration times. Your model should be robust to handle the identical pattern. Holes that hang "out in space" will fail an identical pattern. But my personal opinion is that we've become lazy and just use general for everythijng... I like the speed boost of indentical.

I hope that makes sense but if not, just write back.

Thanks!

-Brian