Advanced round/radius between intersecting curved surface

[PC98]

Hello all!

I am reverse engineering radial pump rotor. I want to achieve a constant radius between pump vane and the ''casing'' - as if it is a ''round'', that fails if I try generating because of complex edge and surfaces. So basically I am asking for help/advice/past experience with how to make complex ''round'' feature on spiral-like intersection of two curved surfaces. I did it before with ''solidify'' of created quilts -but they were uneven and hard to change if I wanted different and constant radius along the intersection.  

Thank you!

[KenFarley]

Things I've resorted to in order to get rounds like this to work:

(1) Put in a very small radius round, then keep increasing it to see where the "choke" point is on the geometry. Looking at your images, I'd guess it's probably at the vane leading or trailing edges?

(2) Maybe try putting rounds on the leading and trailing edges of the vane first, then put the root and tip rounds in. The geometry of a round that goes around a sharp corner is pretty messy, especially when the surfaces are complex like what you're showing. Plus, an actual vane in a part like this, which is usually cast, is not going to be a sharp edge, so it's more realistic to have a radius of some sort. This might make it "easier" for Creo to calculate the geometry.

(3) If the part is going to be made by having some sort of machining that cuts off some of a round, I will model the thing with extra width/diameter, etc. then do a cut to remove the excess. I always try to do the models so I get the true configuration of the part. It's more features, but then again, usually more stable and modifiable.

[PC98]

Thank you, Ken. The main problem I am facing now is, that the curve where surfaces meet, stops round from having greater radius. Round does not want to cross over to the next surface (middle part of the vane). 

[tbraxton]

We need to understand why a round is failing and that is not understood from your post. There are other considerations that can affect this not related to the round feature as well.

If you can post a model with the geometry in question, that will likely result in better feedback.   Note what version of Creo you are using and put the part in a zip file before uploading it here.

[PC98]

Hello,

file is attached (I am using Creo 10.0). Leading and trailing edges will be done later on. But for the sake of my understanding how to solve this problem there is this 'playground version', where I struggle to make my wanted round with radius (R=8 mm). The idea is that it is made in a way that I could change it later on if needed. I have done a round on one side of the vane, but it can not be made any bigger, since I run out of ''extruded material'' (which I have made from the main middle part of the vane, so I can put round on it-- *on attached picture it is coloured in green*). That means that the solidify with which I made vane intersect with casing, is not exactly defined, since it is made just for the sake of the ''round''.

In short: I am unable to make round (that is currently done on the vane root) have greater radius (for example R=8 mm).

Thank you!

Best regards,

PC98

[tbraxton]

These boundaries will be problematic with the application of rounds. The red boundaries are only position continuous (G0). The orange boundaries are tangent (G1) continuous. The math across the boundaries is not "clean" for lack of a better term. For an impeller blade I would target G3 continuity in the radial direction for functional reasons (flow).

You have a patchwork of surfaces that are used to create the blade and fundamentally the way it is built is likely to cause problems with model stability and things like rounds. The internal ids for parents of the round change as the radius increases and some geometry likely is indeterminate when applying the round.

Ideally you would build the vanes such that they have G2+ continuity across the entire face a seen in the picture below. Try using a variable section sweep or other method as applicable to create the vane surfaces such that you have one continuous surface and not a patchwork of quilts.