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Adding fillet that intersects an edge

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equiaxcrystals

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1777334150113.png
Hello!

I am struggling with this certain design. I have a lofted feature that's bottom is extruded into a revolved feature. I want to add a fillet at the base of this, but the small face created from the extrusion off the loft will not allow me to since it intersects the lines. Does anyone have any kind of work around or way that I can combine these features and get rid of these lines?
 
What are you using Alibre Design or Atom 3D? Reexamine the profiles of the Loft to see if they can be adjusted to accommodate the extrusion bit.
If you have it available to you, you could try Remove Face and see it that will patch the surface so you can apply the fillet.

1777334757618.png
 
HaroldL said:
What are you using Alibre Design or Atom 3D? Reexamine the profiles of the Loft to see if they can be adjusted to accommodate the extrusion bit.
If you have it available to you, you could try Remove Face and see it that will patch the surface so you can apply the fillet.

View attachment 47123
Click to expand...
Thanks for the advice. Unfortunately, the remove faces did not work.

I am using alibre design. I tried to include the extruded bit into the loft, but the feature in extrudes into on the bottom is a revolved feature, and I could not figure out a way to create a sketch on a plane above the revolved feature then some how wrap that around the revolved curvature and then loft from there. I tried the wrap tool, but it only creates a boss or emboss.
 
Another option is adding more material, then boss cutaway/trim back to the target size/shape or make the loft or revolve larger than you need then cut/trim/move face back to your target size/shape.
 
Or re-consider the order of features, do the loft before the revolve - so that bottom of loft gets 'buried' in the revolve.
 
I would love to take a look at that part it the IP is not secret. That edge being so close would appear to me to severely limit the size of fillet you can put on which may or may not be an issue. I think the silver bullet would be to get the loft profiles to make it so that the extrusion is not needed, but I can't tell if that's a feasible approach from here. It may be worth checking the part integrity under Inspect> Check Part to make sure there aren't topology issues that are throwing the fillet off. Sometimes it helps to click every single edge the fillet will go down in order (Solves some stitching problems sometimes). Something that is not advisable and not a best practice is to fillet the upper edge and then fillet the bottom to get the fillet to appear along a smoother area. Stacking fillets like that makes for fragile topology but if your desperate it has been done before. I may be able to think of more if I'm able to see more of the part, but I understand if the IP is secret.
 
Thank you everyone for your interest in helping me out.

stepalibre, I tried this but unfortunately it messes up the geometry / angles of the loft upwards, so I cannot do this.

DavidJ, I also tried doing this, but the edge is still there and messes with the ability to put the fillet it.

Joseph, I made a separate part file that reflects the problem I am having and have attached it. I would be very appreciative if you could check it out. After sitting with this issue for longer, I believe I have a deeper issue than what I originally thought I had.

Basically, I am trying to model turbine blades by each radial point and then lofting them together. The issue with this is that each radial point has a planar sketch, so by the time it reaches the hub, the sketch does not fit the curvature of the hub. What I am really hoping there is a work around for is some kind of way to create a planar sketch as normal, and then project that sketch around a cylindrical plane. That way the sketch could be lofted directly off of the hub to the next radial point, and there would be no edge in the way of a fillet. Also, it would be nice to be able to do this at every radial point of the airfoil as it would make it more accurate. Does anyone think this is possible to do?

Thanks!!
 

Attachments

In addition to Harold, here is my version as well. I'm seeing an infinitely thin intersection between the blade and body. 1777904736147.png

This would be a significant complicating factor for solving. In my upload, I changed the sketch to be .01" different before editing. But I think Harold's solution is the most elegant way to get away from that thin contact. Let us know if these help, I know it's hard to represent a part in more simple terms and still be able to get a usable solution.
 

Attachments

Joseph_L said:
In addition to Harold, here is my version as well. I'm seeing an infinitely thin intersection between the blade and body. View attachment 47190

This would be a significant complicating factor for solving. In my upload, I changed the sketch to be .01" different before editing. But I think Harold's solution is the most elegant way to get away from that thin contact. Let us know if these help, I know it's hard to represent a part in more simple terms and still be able to get a usable solution.
Click to expand...
Thank you, the offset face is exactly what I was looking for! Even with changing the sketch to .001" different it still works out great. Thanks for spending the time to help me out on this.
 
HaroldL said:
So, you want something like this...

View attachment 47172

I changed the Extrude Boss Type to Dual Depth so the blade projects into the hub. Also reconstrained the hub sketch so it isn't driven by the end of the blade.

Now you can fillet between the two features...
View attachment 47174
Click to expand...
Harold, thank you very much for the help. Unfortunately in my simplified part example it doesn't show that I will actually be lofting the airfoil profiles to one another, not extruding them, so the dual depth wouldn't work. That is my bad, but I really appreciate you taking the time to help me out on this.
 
equiaxcrystals said:
Harold, thank you very much for the help. Unfortunately in my simplified part example it doesn't show that I will actually be lofting the airfoil profiles to one another, not extruding them, so the dual depth wouldn't work. That is my bad, but I really appreciate you taking the time to help me out on this.
Click to expand...
Yeah, I wondered what happened to the loft. I figured you must have changed your design strategy to an extrusion.
So, with a Loft are you creating a twist in the blade as seen in some applications? :confused:
 
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