Hi John...
I think you're taking the wrong approach to this particular problem. I've remodeled the part with what is, in my humble opinion, a better technique.
The key to the solution was your statement "What i also require, is for the holes in the second pattern to remain normal to the revolved surface". If you're creating holes and you want them to stay normal to some crazy surface, the first thing you should think it "On-Point Hole". This is a special hole type that doesn't appear on the hole type drop-down menu. The only way it appears is if you select a datum point as the first hole reference... but there's a catch, the datum point has to be an "on-surface" datum point.
Luckily this completely works for your situation.
I remodeled your part and attached it in Creo 2 format. I'm not sure which version you're running... it looked like Creo. I should've created it in Creo 1 but I wasn't thinking when I made it. If Creo 2 doesn't work for you and the instructions below don't help, let me know and I'll remodel in Creo 1.
First... delete the intersection and the second pattern. Next, try this (click each slide for a larger image)...
That should give you everything you needed including all original dimensions. You're able to use a simple hole rather than a revolved one. You're also able to eliminate the hole depth and allow Creo to control it automatically. You don't need the intersection... and you can easily hide the datum points by layer.
Hope this helps!
Thanks!
-Brian
Hi John...
Check out the annotation below... is this the dimension you wanted?
This is a parametric reference dimension created right in the model. It travels with the holes. Also, I reworked the model so everything ran from one pattern. Here's the model tree...
You can obviously still do it the way you were before. For reference, I've included the part in Creo Elements/Pro (Wildfire 5) format. Take a look at the annotation. Here's a quick run-through of how I created this dimension...
- Select Insert->Annotations->Annotation Feature (You can use the new annotation icon, too)
- Select the Reference Dimension radio button and select OK.
- Select Make Line->Horiz Line (as shown below) and select the Datum Point as a reference. You should see a horizontal line appear. If you see a vertical line even after you chose "Horiz Line", never fear. We can edit it later.
- Select On Entity from the menu and choose the Axis as shown (axis is in red), horizontal line shows up in purple on the image below.
- Press Middle Mouse Button to "Drop" the dimension as shown.
- Use Edit Orientation to achieve the correct placement and rotation for your dimension. It takes practice but within a few minutes, you;'ll be an expert.
Hope that helps!
Thanks!
-Brian
