Relations: within sketch or feature assigned (?)

[TomD.inPDX]

We have a couple of options when we want to create associativity between features.

Question for your first go-to solution:

Do you place the relations within the sketch or do you assign relations holistically at the feature level?

I'm sure there are implications both ways.  If you have something to add, please do.

I did notice that sketch relations take priority over feature relations.

Features with sketch relations and feature relations affecting the same dimensions means that the feature relations are ignored.

I see no warnings that there are two relations tied to a dimension.

In general I always thought relations assigned within the sketch were easier to manage.

Now I am second guessing this belief.  Your thoughts?

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[dschenken]

Model relations are certainly more discoverable by the average user.

If the dimension record for the sketch and the feature is the same one, then they just failed to create a check for interference. I'm guessing they aren't the same record or they use two different links to the same record, which is why the software isn't capable of noticing without a much larger effort.

Mostly I use sketcher relations to force shape into place; especially when a lot of relations are required so that it doesn't overwhelm the feature/model relations that are to drive function (such as centering, or making margins equal)

[TomD.inPDX]

Model relations are easy to find but that screen gets messy fast.

Right now I only have 4 relations at the model level driving the design elements requires.

I started editing feature relations and found that to be very cumbersome.

Then I started adding them to the sketch itself and learned the sketch takes precedence.

So of course, had to go back an remove the feature relations.

In past designs I've ended up having to regenerate twice to have everything catch up.

Often times, Creo doesn't want to regenerate the second time because it thinks it is done.

Yet, you know there is a feature that will change if it does regenerate as it should.

That is part of what prompted me to ask the question.

I do know about Initial and Post Regeneration option in Relations but that is only active at part levels relations.

What I haven't found is the logic of when things require 2 regenerations.

And does that have anything to do with this query?

[dschenken]

Multiple regens required is a sign of a circular reference; that is, that some output along the way affects some earlier stage. Unlike ordinary circular references, Creo does not report a certain class of them as an error. I think it only indirectly discovers them because at the end of regen some item is flagged as changed after dependencies based on it were made.

Why Creo fails to regen when it should has been a mystery to me; I've written before that I think it is speed optimizations that skip a few cases they should not. Excel has the same sort of issues, but has much easier dependency trees to deal with. Even then, Microsoft gives up their optimizations beyond a certain size.

[BenLoosli]

I use relations at both levels depending on what may need to be changed.

When creating hardware items, like screws, I will put an end chamfer on and use a sketch dimension for the length and then set that to a percentage of the thread diameter. No need to ever go in and change this value.