Why is this weird edge happening when I create a chamfer? This is a section view, it is a full circle.
The two faces are parallel with a normal distance of 0.06 in.
Why is this weird edge happening when I create a chamfer? This is a section view, it is a full circle.
The two faces are parallel with a normal distance of 0.06 in.
Can you be more specific with your question? It just looks like a cylindrical hole that you did not complete the chamfer for. I noticed that this was a pretty small hole however and so you may be seeing a graphical problem where the rendering does not show exactly how it should due to the small size. You can try increasing your image quality to see if that helps.
Sorry, this is a cross section. It is a full circle. The preview looks exactly the same as the final chamfer. I don't think it's a graphical issue as there is a face still present. There should be no face here. That is the weird edge I am referring to.
Can you upload the part so we can try to reproduce this ?
If you are able to select it I agree that the geometry seems wrong in this case. Could you upload the file so that we can see what is causing this?
Looks like your top face and bottom face are not parallel
They're parallel. See the second screenshot showing they are in the measure tool.
I added it to the original post.
Sure, I added it to the original post.
I see the same thing, but cannot explain it.
If you place a plane on the top face, and then another at the top of the chamfer, it says the angle is 1.9 degree.
I also tried exporting it as a parasolid and then reimporting it. No change.
The top and bottom of the box are 2 degrees off.
The sketch for your extrude cut is on the bottom face, but the "from" is the face at an angle. The extrude vector is from the bottom face, not the top. So even though the faces are parallel, the cut is not perpendicular to those faces.
Fixing the extrude vector in the cut solves the problem.
OK. I have no idea what you are trying to do here.
You're either doing this on purpose, or [deleted].
The top and bottom of the cut are indeed parallel, but the axis of the hole is not perpendicular to the face because you drew the sketch on the opposite side to the angled face. The hole edges (top and bottom) are not circles but ellipses. Since you've selected an angle-distance chamfer, and the angle varies due to the skewed hole axis, your chamfer doesn't extend to the rim of the hole on the uphill side.
You need to define what you actually want out of this feature.
Is this?
The planes are parallel, but the top surface is at an angle of 92deg. I changed this to 100 so that you can see the difference better but as you can tell this will affect the chamfer.
The cut is exactly how it should be and made that way on purpose. This is a molded part and the hole needs to made in the direction of pull (normal to the top plane).
The chamfer still shouldn't do that. Both faces are parallel so the chamfer should be 0.06 at every point around the diameter.
Yes, the hole is made that way on purpose.
I understand about the axis, but if I change the chamfer to D x D and use 0.06 for the first dimension, it should always reach the top surface, shouldn't it?
The top and bottom faces being parallel is not the determining factor for this case. the angle of the side wall and the top/bottom faces is what determines this shape. This currently is functioning as intended.
Assuming you didn't change the direction of the extruded cut or angle of the top surface, yes that is what it should look like.
Josh Helman wrote:
The top and bottom faces being parallel is not the determining factor for this case. the angle of the side wall and the top/bottom faces is what determines this shape. This currently is functioning as intended.
Where your purple arrows are, both sides are 0.06 in. If I change the chamfer to D x D, and use 0.06 in for that dimension shouldn't it always reach the top surface?
I continued from where you left. It is mere patch up work, not being try to find out why chamfer does not work.
Well, I have the geometry I want using a neutral plane draft feature, with the top surface as the neutral plane.
I'd really like to understand why when using a chamfer if isn't using the dimension all the way around though.
The top edge of the chamfer should not move, when I change D2. But you can see when I lower D2, the top edge of the chamfer moves closer to the top surface.
David Lane, the .060 dim on the distance chamfer is NOT measured ALONG the edge, but rather perpendicular to the opposing face.
or I might have that backwards - not much caffeine yet
If it's 0.06 from the bottom face in a perpendicular direction, it still shouldn't move when I change the second value. It really shouldn't be from the perpendicular though.
This image shows it's measured from the two faces that insect to create the edge. They shouldn't have to be at 90 degrees from each other for it to work properly.
Try creating the chamfer manually, using a sketch and a sweep. I haven't done this, but i'm guessing the challenges of that geometry will become apparent if you do.
It's a functional limitation. Theoretically, you're correct. However, the chamfer function doesn't work like that in its underlying algorithms. The angle between your two faces varies continually. Yes, at every point around the ellipse it's possible to measure off 0.06 along the face perpendicular to the ellipse at that point. But that would be a significant increase in complexity to calculate. A simple chamfer can't chamfer properly between two faces whose relationship is continually variable like these.
Here's another example... It's a sweep with a twist-along-path that intersects a flat face, creating a continually variable relationship between the two faces. It's a distance-distance chamfer, symmetric at 0.02 per leg. This 0.02 per leg measurement is correct at the center. However, due to the way the algorithm works, it doesn't end up measuring correctly at the ends. It's ballooned out to 0.03 at the 90 degree end, and shrunk to 0.012 at the 135 degree end. Somehow it does seem to maintain the offsets as equal, but doesn't maintain their value.
Is it a bug? I dunno. Probably more like a limitiation. I have no idea how the underlying geometric calculations are done, but I do know that the surface you're actually looking for is not a simple one.
It's a functional limitation. Theoretically, you're correct. However, the chamfer function doesn't work like that in its underlying algorithms. The angle between your two faces varies continually. Yes, at every point around the ellipse it's possible to measure off 0.06 along the face perpendicular to the ellipse at that point. But that would be a significant increase in complexity to calculate. A simple chamfer can't chamfer properly between two faces whose relationship is continually variable like these.
Here's another example... It's a sweep with a twist-along-path that intersects a flat face, creating a continually variable relationship between the two faces. It's a distance-distance chamfer, symmetric at 0.02 per leg. This 0.02 per leg measurement is correct at the center. However, due to the way the algorithm works, it doesn't end up measuring correctly at the ends. It's ballooned out to 0.03 at the 90 degree end, and shrunk to 0.012 at the 135 degree end. Somehow it does seem to maintain the offsets as equal, but doesn't maintain their value.
Is it a bug? I dunno. Probably more like a limitiation. I have no idea how the underlying geometric calculations are done, but I do know that the surface you're actually looking for is not a simple one.