I am new to Creo and have been trying make a model of a human hand. I have different sketch profiles to make up a finger (see attached) and want to boundary blend the entire profile. I believe I'm misunderstanding something about the feature since there is nothing really complicated about my sketches. Any thoughts?
I don't have Creo 4 loaded so this I file cannot see.
Boundary blend requires some finesse. While you pick you boundaries, it appears to assume a start for each segment. If these segments are rotated where the paths cross, they tend to fail the feature.
This is just one of many things that can happened but for the most part, you have time within the dialog to correct whatever needs correcting.
This is one of those commands that you could build an entire career around. And you are right, they make great single feature surfaces with amazing flexibility. It is just that it is so poorly understood, or even documented that it is very much overlooked.
If your problem is rotational relationship with the prior element, just highlight the chain under the Curves tab and it will show you a white dot. Highlight the next and the white dot for this one should be in a rational position according to the first. If not, just drag the white dot to where you want it to be. Once they are all aligned, hopefully a surface appears. Next you get the options of tangency or curvature. This is where things can go very wrong again. However, you get to select you tangencies in the constraints tab. Control over these is not for the faint of heart when it comes to 1) being successful and 2) keeping your design dynamically flexible. The third tab is Control Point which again, is very powerful and should have some elementary background as to what they do, but the short of it is that this is where you can make specific connections. The 4th I rarely look at but it has even more functionality for the purposes of influencing the surface.
You can use a single or dual array. Know that a point feature as the second "chain" is valid.
Closing up contoured voids with boundary blend is near impossible... gets touchy, to say the least.
Core Creo surfacing features are not known for high quality surfaces. The system is not forgiving in the least. It does exactly what you told it to do, with all its consequences.
Hope some of all that helps
Don't forget to find the allow_anatomic_features yes so you can access some of the older surfacing features. They have a maddening interface but they also solve some thing you will want. 5-sides fills (N-sided Patch) for instance is a hit with some old timers here... old ...old old... you know who you are.... Frank
Your smaller elliptical curves aren't connected to the larger longitudinal curves. They all have to touch in order to fully define boundaries. And when you redraw them you only have to do one half. Since your finger is symmetrical you can then mirror.
Sorry for the late response. Thank you, gmcmurray for bringing that up. I just noticed that my reference lines are not letting me make the points coincident with my oval sketch (see pic attached). As mentioned, I am very new to Creo. What's the quick fix for this?
Ahead of your sketch create a datum point at the intersection of the sketch plane and the ellipse, then align your sketch to the point. Creo does not have the "Pierce" constraint that you may be familiar with if you've used Solidworks, so you need to create the point at the intersection ahead of time.
Took your advice and still nothing! I notice that the preview of the Boundary Blend will stop once I click the fourth side profile. It doesn't matter which order I pick them in, it always stops showing the preview after the last one. (See attached)
Thank you for your time!
First, I'd try to build this in smaller pieces. At least in half, but perhaps one vertical segment at a time.
Second, when I try to build half, it's giving me an error that the curves don't form a loop, even though when I measure the vertexes they show zero distance between them.
Here's what I tried to build:
And here's the error:
I don't have time to spend diagnosing further, sorry. I'm guessing that trying smaller pieces will help determine where the issue is.
Organic surfacing is not simple stuff, issues like this are not uncommon.
I am having the same problem with Creo2. If you define the boundary blend in both directions, it doesn't like the closing point feature. Change that point to a circle and it will resolve. Then you will need a patch for the tip.
These kinds of closed boundaries have always been problematic for core-Creo/WF/Pro|E.
I still think this is so that you will buy the extension. Or drive yourself nuts with Solidworks instead
Creo 2.0 commercial version attached.