Circular/linear patterns & Mirror

[Dodge]

I'm experienced in CAD, but new to CREO.

I'm finding all sorts of tutorials for how to make a circular or linear patter with a feature such as an extrusion. However, am I able to make a pattern out of just a sketch so that I may later extrude the entire pattern?

If so, do you know where I can find a good tutorial for this?

While we're on the topic, can you do this same thing with the mirror feature?

I know it's possible to do both of these things before and after finishing a sketch in a variety of other CAD software's, but is that not the case for CREO?

[KenFarley · Accepted solution]

Creo does not provide a means of patterning geometric entities within a sketch.

You can pattern a completed sketch. The only times I've done this is when I wanted to have reference geometry for features.

Generally speaking, the emphasis in Creo seems to have been on patterning features. Make a simple (or not) initial extrude, revolve, etc. Then pattern that to get the grid, circular array, etc. that you need. There are a lot of different ways to pattern things, some of which are pretty sophisticated.

To be honest, unless I intend to use a sketch for multiple features, I don't see the usefulness of making a sketch, then making the feature. It needlessly doubles the number of things in the model tree with no obvious advantage. I think the only reason people are taught this method is because that is how it is done in other software. Not a compelling reason.

As far as mirroring goes, you can mirror things in a sketch, I don't know if it's required in the latest versions, but I always use a centerline to mirror geometry in this fashion. They are also extremely useful to define symmetric geometry. You can mirror features, too, but I try to limit that to only when I really need it. Again, I don't know if things are better in the latest versions of Creo, but feature mirroring has proven to be kind of quirky in the past.

[Dodge]

Unfortunate, but I guess CREO makes up for this with a very user-friendly copy/paste mechanism.

Thank you.

[rreifsnyder]

You should also be aware of Geometry Patterns. Using a regular pattern, the entire feature is replicated, so the sketch and extrude/revolve/whatever is entirely created. The problem is when there are lots of instances in a pattern, this can be very slow because after each new feature is created, Creo does a thorough verification that it has ended up with valid geometry, then has to do it again for EACH instance in the pattern. A Geometry Pattern basically does a surface copy (can be more than one feature) of what you want patterned, patterns the surfaces, and THEN does a single feature to add or subtract geometry (it can't do both in one GP). That is doing then a single verification on that, technically single feature.