How best to constrain sketch at a multiple convergence?

[pimm]

When there are multiple entities that come to a convergence it is difficult within a sketch to have the entities move in a reliable manner with changes.  It is also difficult to know which constraints apply to which entity.

Maybe this is really simple but it drives me nuts.

Below is an example of a sketch convergence.  Note that there are a number of point on entity constraints.

converge

There are at least 3 point on entity constraints as well as the point which gets used down stream.  The magenta vertical line is a construction line.  I need to be able to fix the convergence at the horizontal reference.  The center point of the 2 angled lines needs to be at a distance from the vertical reference.  The 2 angled lines needs to have their value driven from the central vertical reference.

What would be nice is if everything that is converged only had one point of which the 2 angled lines only could move in the horizontal direction fixed on the horizontal point held to the horizontal reference.

Is there a simple way of doing that?

[tbraxton · Accepted solution]

Add some construction geometry to define your intent within the sketch. Try adding the construction circle and/or the sketch csys as shown below. You can also lock dimensions in the sketch as required to get desired behavior when flexing the dims.

Add construction geometry

[pimm]

Tbraxton:  This is actually would be 2 viable solutions that would hold geometry in place in my situation.

The use of a circle with same size construction lines from a center point should hold multiple lines to a center point.

Also; I've never used a sketch csys before, but it does appear to keep minor constraints to a minimum.

Thanks, I will be trying both of these ideas as there are different conditions which 1 might be more useful than the other.

[pausob]

Agreed! the computer is pretty dumb when it comes to reading my mind.  I find it's best to spell out every detail in order to provide the system the information about my design intent.  Even then, it will often act strangely when I try to "flex" a sketch 🙄 but I learned to accept that I can't argue with math and I try harder to spot the constraint or dimension that is causing me the trouble.

I'd like to add couple of points with regards to constraining sketches:

1) make it a goal to create a sketch where the number of driving dimensions is minimized - by using constraints and constraining to construction geometry

2) sketch coordinate system is fantastic for "anchoring" your sketch.  Also, you can mirror / impose symmetry constraints about its axes

3) sketcher_diagonal_constr yes may be a good config.pro option for creating line segments at 45° (eliminating the dimension or the 2 equal-sized orthogonal construction segments).  If the above option is active as you are sketching, the system will add the constraint (it's actually kind of annoying on many occasions 🙂

4) select a constraint to highlight it, then right click and "Explain" to gain better understanding.

5) lock your driving dimensions that you know are not meant to "flex".  In the example from the original post, locking the 2 angular dimensions would solve the problem.

There are so many other things to know and learn about the sketcher but I am not trying to turn this into a sketcher "tips and tricks" discussion.  Again, I want to emphasize point #5 above.

[pimm]

Pausob:  Even though I've learned a lot about constraining sketches in general I came from a background of not using them before so I have a few holes in my understanding of Creo's constraint system.

You've given another thumbs up for the sketch coordinate system.  To know this can be used in mirroring really lets me know I have to start using this.

I do agree that sketches need to be locked down to prevent them from unraveling them.  In this case the 2 angles are actually locked.  It is only the origin point at the convergence that was open.  In general locking down sketches in our line of work is not easy as we will have hundreds of curves, lines and arcs in a typical sketch.  Sometimes we leave the original sketch as is and reference this in another sketch that gets some tweaks.