Can I automatically suppress multiple features at one time within Creo? For example, can I define a rule that says to suppress all holes with a diameter of 6mm or less?
Explore the search tool.
You can create a search with two rules, the first select all the hole features like shown above:
the second rule select the ones that have the pretended dimension:
You can save this query too for later use.
Explore a little this tool to see how powerful it can be.
Another option is to create a layer with the previous rules, then you just have click on the layer, "select items" and "supress".
I found recently that is possible to copy layers from one model to another, this is really handy because you can have a model with all these layers with associative filters and just copy paste it to another.
Can you please confirm that "AND" works correctly is this specific case? In Creo 3 M050 it seems to be ignoring the "AND" and treating the compound query like "OR".
After some more tests, I realize that the "and " operator doesn't always work, sometimes the results aren't the expected...
Anyway, for this case, I played a little more with the tool and isn't easy as I expected. I could make it work but not in a very elegant way....
First create a new layer (example "holes"), create rules for it and make them associative.
I had to create 3 rules to make it work:
The filter is on, now select only the features in layer tree (don't select the dimensions), switch to feature tree, RMB-> Suppress
There might a cleaner way to do this, but this is the best I achieved.
Not easily, and not without advance planning. If this is a model that you have full control over and want to build automation into, then yes. If you simply want to open anyone's model, locate fasteners by size, and create a rule to suppress, then no.
Here are the steps to automate with Pro-Program:
Example (d18 is the hole diameter):
IF D18 > MIN_SIZE
ADD FEATURE (XXX)