I am working on a round feature that I have been quite unsuccessful in creating. I believe I understand the problem but I am not sure how to fix it. Any help would be fantastic.
I am creating a round that has a R.060 and once it gets to a point where it doesnt have the needed .060 vertically, it fails to propogate. What is the best way to create this feature so that I have a constant width radius?
This is one of those cases of trying to model a material removal artifact by adding material. Obviously you can see the problem. An alternative is to create the material removal feature as a cut representing what a mill-turn machining operation will do using a variable section sweep. Set up a trajectory curve that spirals up the basic cylinder and cuts material away. This will avoid the glitch you are going to get if you were able to complete the round you are trying for.
I don't know the intricacies of your model, but my approach with these types of things is to build the protrusion taller, put the rounds on it, then cut it back to the final height above the cylinder. You're likely having trouble because the radius you're putting on the round is *exactly* the same or slightly less or more than your protrusion height, and Creo is having mathematical troubles with it. It causes a topographical discontinuity, perhaps.
If I'm looking at the problem to simplistically, sorry. It's hard to discern what is a possible solution given just a picture and not knowing the design intent, etc.
Try selecting the "intent feature" for the corner-edge.
In early Creo 2.0, there is also a bug in continuous helical geometry.
I'll elaborate if needed.
I also like the concept of maintaining a larger diameter of your shaft and trimming the diameter after establishing a successful round feature. If this functions, then you simply ended up with one of those parts that wants to be difficult.
The topological difficulty is that it transitions from a Surface-Surface round to a Surface-Edge round.
Basically, the cutter is falling off the helical face of the part when that face is too narrow to stay completely on it.
If Creo did handle it it would have to prompt the user to determine if the transition should be a radius pivoting around the end of the edge or a miter with a sharp intersection between the rounds on either side of the end of the edge.
Okay, fair enough, David.
I've had pretty shaky results with rounding things for 3D printing.
Sometimes they work and most times they don't.
And they often get in the way of revisions that cause the round failures.
When a solid won't regenerate, a surface may work instead.
One other trick that might work is to make the round a surface element first and manipulate that to later generate a solid using the Solidify feature.
Thanks for the reply.
Unfortunately, when making it large and then cutting away you end up with a thickness across the flat portion of the flight that is varied a small amount. This does work but I want to control the width more accurately.
The description of the issue is what I believe to be correct. I have tried transition mode with several selections and settings to solve but have had no luck.
Thanks for the reply
That does complicate things.
That widening you are talking about is a consequence of the "assumed" tool path along the inside edge (corner). Your desired toolpath will have a deviation when the tool leaves the outer edge. If you define that refined toolpath, you can use a sweep/cut along the toolpath to attain the round exactly as you want it.
You can try to create 2 sets of rounds: one with surface to surface for the major portion and another one with Surface to Edge at the end, and then you can create a transition between these two sets.
Without actual model its difficult to say what works