Correcting a bad curve

[ianhughes7UFVF]

Hi

I am trying to recreate a project from pdfs that have really specific curves to create.

What I was using is this for example:

As you can see the top curve is made from 3 radius' and then joining the three together creates the curve. When I did this and converted it to 3d I got two joins reflecting the three different curves.

So the curve has dimples as it were.

I tried using a spline but that seems to create an inaccurate curve too. An eclipse doesn't fit nor does a set of arcs.

Is there a way of cleaning up the  3d fusion curve so that the curve flows neatly.

I have attached the file for you to look at.

Kind Regards

Ian

[TheCADWhisperer]

In my opinion your sketch is far more complex that required.

I suspect that you are missing some Tangent constraints in there.

Many of your dimensions do not make logical sense (not measurable in the real world).

Edit:  Oops, I see you are converting from inch to mm that might account for some of the "oddball" dimensions.

Can you Attach the original pdf from your image?

[Oceanconcepts]

Having three different radii in the curve will necessitate some kind of joint between them. You could make a sketch with the three radii and fillet the arcs where they join, and introduce yet another set of radii. But what’s going on here? It seems like a very odd way to define a curve, and of necessity defined this way it won’t be fair. Should this curve really be a conic section? 

[g-andresen]

Hi,

1. All I see here is a collection of radii. So they are all not defined because they lack the start and end points.
2. If splines don't give the desired curve, it's mostly because you have set their control points with the corresponding tangents wrong and/or the amount of control points is not favorable (mostly too many).
The problems with the conditions have already been mentioned.

If a true-to-scale template exists, only the controlled tracing with splines remains.

günther

[ianhughes7UFVF]

Hi,

Thanks for the responses.

The sketch I created is based on a pdf that was done in a way that I appreciate I wouldn't have used myself.

I am sure there would have been a better way of doing it. The original sketch was based on measuring an original 60s prop part.

I have converted to mms from inches but kept the decimal places rather high to keep the inches accurate.

I did try a spline, but I kept on forgetting to go across where the circles meet and continued the dimple effect.

I have attached the pdf that I used if that helps with finding a neat solution to the problem.

Kind Regards

Ian

[ianhughes7UFVF]

Hi

Would you suggest that I redraw the whole sketch in inches too.

I am so unuse to using inches being in Australia, I always convert to mms to about 4 decimal places.

Kind Regards

Ian

[Oceanconcepts]

No reason I can see to use inches- I'm in the US and do 99% of my work in metric, which is the native system for Fusion. 

I opened your sketch and can quite easily get a quite precise fit to those curves using a spline curve with a single control point . If you goal is to have a smooth face without breaks that is very close to the dimensions described then that would look to me to be the best way to get there. The most common problem with using splines is to use too many control points, you want the fewest you can get away with. 

If it is vitally important to have those precise radii at specific points, then you are going to have some transitions between faces. While you can have continuity with the curvature so there are no edges, the curve won't be what in my boatbuilding world we would call "fair". It will be lumpy. 

It depends on your end goal. 

[ianhughes7UFVF]

Hi

I appreciate the comments on inches and metric.

What I thought I would do is switch the sketch to inches and then make sure all the measurements are as per the pdf.

But it sounds like the spline is the way to go.

When I tried, I was doing very little distances between points which obviously wasn't helping. I can give it another go making the jumps further.

Kind Regards

Ian

[Oceanconcepts]

Yes, you can match that curve very closely by placing a spline point at each end and using one control point- a single spline segment. I don't know the source of the .pdf obviously, but it looks like an attempt to describe in terms of arcs a curve that was probably a faired spline in reality. In the old days (which I am old enough to remember) one might describe shapes in that way in blueprints, and leave it up to the old guys carving patterns out of sugar pine to do the actual fairing.  😉

[chrisplyler]

Your arcs are not tangent to each other.

Watch me fix it. I deleted stuff in your sketch that was distracting to me and didn't seem to serve a purpose. I chose to dimension in inches since that is what your drawing has.

In Model workspace, the lines will still show at tangencies, but as you can tell when I go into Render workspace, it is a smooth surface.