How do I make this part?
Forum rules
and Helpful information
and Helpful information
IMPORTANT: Please click here and read this first, before asking for help
Also, be nice to others! Read the FreeCAD code of conduct!
Also, be nice to others! Read the FreeCAD code of conduct!
How do I make this part?
Hello. I'm new to freecad and I have two of these parts to make. One an oval, and one an odd shape. I've managed to make the oval one with the curved surface add on, but am having trouble with the other one. The first one I simply make the oval on the xy plane, a thin curved oval on the xz plan and a shorter one on the yz plane. When I do this with the other part, I get a lot of weird things happening if anything at all. I also can't figure out how to fillet the corners on the two holes because it is on a curved surface. Any help would be greatly appreciated.
- Attachments
-
- dgv.png (184.45 KiB) Viewed 1759 times
-
- Version B.pdf
- (231.45 KiB) Downloaded 26 times
-
- Version A.pdf
- (229.23 KiB) Downloaded 52 times
- thomas-neemann
- Veteran
- Posts: 11958
- Joined: Wed Jan 22, 2020 6:03 pm
- Location: Osnabrück DE 🇩🇪
- Contact:
Re: How do I make this part?
Here's a quick and easy suggestion, I can make a video for you if you'd like
Re: How do I make this part?
The dimension between the holes is missing.
Attached an example in PartDesign.
Attached an example in PartDesign.
- Attachments
-
- elipsoid_OB.FCStd
- (108.38 KiB) Downloaded 29 times
Re: How do I make this part?
Another quick and easy way is to clone a sphere and apply differential scale ratios to each axis, subtract cylinders or extruded circles for the holes.
Re: How do I make this part?
Thanks for the reply. That does let me fillet the holes which is great. The only issue with an ellipsoid or scaled sphere is that they make the part with a smaller radius along the outer oval, which is why I had to used curved shapes. I don't believe there's a way to increase the size of that sharp radius of an ellipsoid. What do you think? This may be okay for who I'm making it for though, I'll have to find that out.
I've already 3d printed this part, and I made a tumbler using a folders can,10 dollar motor and other parts to round the holes of the 3d printed part physically. Just waiting on tumbler media to use it. I'm not sure how that will work out yet but we'll see.
My biggest conundrum is the attached "Version B". I'll attach it again here. It's not an oval so ellipsoid or scaled sphere is a no go. I'm assuming curved shapes is the only way to manage this. Do you think it's possible? A video of this would be awesome. Thanks.
- Attachments
-
- Version B.pdf
- (231.45 KiB) Downloaded 31 times
Re: How do I make this part?
shapes like this is something that looks simple but often turns out to be a pita to get done.
in short, not everything is possible in fc at time of writing (at least through gui).
double curvature surfs is a tricky area for any cad sw.
there are of course different attempts to improve this,
curves, nurbs and silk add ons are examples of this.
best bet for shaping complex freeform surfaces is gordon in curves wb.
when surface wb works - which it does for a lot of things,
it is quick and easy to use, however it does not have edge tangency
which limits the overall usability.
same goes for sketcher, in v0.19 there is no tangency/point on curve
for splines - this also makes things more tricky to work with sketches for freeform surfs.
curves wb can be used to work with tangency of splines.
here is a file with some different possible techniques
none of them is particularly good. if one accepts G0 surfaces, surf wb and a bit of carving with sweeps is a fairly easy way to go.
making gordon surfaces properly means quite a bit of ground work to be done.
gordon seems to always work when using 4 boundaries, but at the same time for a
shape like this 4 boundaries is not enough, as shown in the file.
it is not a given that gordon works when adding intermediate guides (at least not for me).
the 2 options in surf wb behaves quite different on the same boundary curves,
the option in which extra edge boundaries often gives degenerated surfaces,
so usability of that one is limited to simple surfaces.
in this case the surf wb option that worked for me was the one without edge constraints.
if someone would like to take a stab at this with nurbs / silk that would be interesting to see the outcome of.
in short, not everything is possible in fc at time of writing (at least through gui).
double curvature surfs is a tricky area for any cad sw.
there are of course different attempts to improve this,
curves, nurbs and silk add ons are examples of this.
best bet for shaping complex freeform surfaces is gordon in curves wb.
when surface wb works - which it does for a lot of things,
it is quick and easy to use, however it does not have edge tangency
which limits the overall usability.
same goes for sketcher, in v0.19 there is no tangency/point on curve
for splines - this also makes things more tricky to work with sketches for freeform surfs.
curves wb can be used to work with tangency of splines.
here is a file with some different possible techniques
none of them is particularly good. if one accepts G0 surfaces, surf wb and a bit of carving with sweeps is a fairly easy way to go.
making gordon surfaces properly means quite a bit of ground work to be done.
gordon seems to always work when using 4 boundaries, but at the same time for a
shape like this 4 boundaries is not enough, as shown in the file.
it is not a given that gordon works when adding intermediate guides (at least not for me).
the 2 options in surf wb behaves quite different on the same boundary curves,
the option in which extra edge boundaries often gives degenerated surfaces,
so usability of that one is limited to simple surfaces.
in this case the surf wb option that worked for me was the one without edge constraints.
if someone would like to take a stab at this with nurbs / silk that would be interesting to see the outcome of.
- Attachments
-
- smoothstonea.FCStd
- (835.68 KiB) Downloaded 22 times
Re: How do I make this part?
with Silk, make sure to use the ControlGrid44_Rotate tool (next to ControlGrid44, no specific icon)
Because we are only going to feed in 3 edges, this control grid has a degenerate edge, but assumes it will be used in symmetry (this is how a nurbs sphere is usually done)
To get the degenerate point in the center pick the control polys in this order in this order: center to long edge, then perimeter, then short edge back to center.
the Silk related stuff goes as follows:
-3 ellipse sketches (FreeCAD)
-convert each sketch to a ControlPoly4 (Silk)
-pick the polys in the order described above, then ControlGrid44_Rotate (Silk)
-apply a CubicSurface_44 to the grid (silk)
-Part>mirror a bunch of times. some surfaces appear black, combo view > view > lighting : two sided as a temporary fix (FreeCAD)
-Part>Shape Builder ("advanced utility to create shapes") > make a shell (FreeCAD) this conveniently ignores that some faces were inside out
-same as last tool > shell into solid (FreeCAD)
-some random booleans or whatever (FreeCAD)
Because we are only going to feed in 3 edges, this control grid has a degenerate edge, but assumes it will be used in symmetry (this is how a nurbs sphere is usually done)
To get the degenerate point in the center pick the control polys in this order in this order: center to long edge, then perimeter, then short edge back to center.
the Silk related stuff goes as follows:
-3 ellipse sketches (FreeCAD)
-convert each sketch to a ControlPoly4 (Silk)
-pick the polys in the order described above, then ControlGrid44_Rotate (Silk)
-apply a CubicSurface_44 to the grid (silk)
-Part>mirror a bunch of times. some surfaces appear black, combo view > view > lighting : two sided as a temporary fix (FreeCAD)
-Part>Shape Builder ("advanced utility to create shapes") > make a shell (FreeCAD) this conveniently ignores that some faces were inside out
-same as last tool > shell into solid (FreeCAD)
-some random booleans or whatever (FreeCAD)
- Attachments
-
- ellipsoid_01.FCStd
- (81.5 KiB) Downloaded 23 times
Re: How do I make this part?
as mentioned, this control grid works best when there is symmetry involved (it wouldn't necessarily connect well to a random surface.
this loss of general connection has a payoff: the degenerate corner is pretty smooth
this loss of general connection has a payoff: the degenerate corner is pretty smooth
Re: How do I make this part?
unfortunately, FreeCAD cannot fillet the edges of my boolean cuts
bummer, this limits the usefulness of the technique. In the models above, it appears that the successful fillets are on planar faces. Is that true?
The advantage of the technique is that i get exactly the base shape i want with the absolute minimum number of control point on the surface, which keeps the model nice and light.
bummer, this limits the usefulness of the technique. In the models above, it appears that the successful fillets are on planar faces. Is that true?
The advantage of the technique is that i get exactly the base shape i want with the absolute minimum number of control point on the surface, which keeps the model nice and light.