I'm modelling a Haack Series Nose cone. The nose cone equation for the curve is:
This is the equation for the datum curve that I have in Creo thanks to the people who helped me in a previous thread where I could not get the equation to draw near the bounds:
R = 49
L = 560
z = t
y = ( R / sqrt ( PI ) ) * sqrt ( ( acos ( 1 - ( 2 * t / L ) ) ) * pi / 180 - sin ( 2 * acos ( 1 - ( 2 * t / L ) ) ) / 2 )
x = 0.0
So here is the problem: zooming in where the observed segment of the curve spans about 10 mm of length, there appears to be a small concave segment and the tip seems to blunt abruptly:
The gradient should always be decreasing, yet by visual inspection and the curvature analysis tool, we can see this is not the case.
This is how the shape should look:
I've attached an excel plot of what the values should be for the length of the cone. Creo more or less agrees with the numbers until it gets within less than 20 mm of the tip where the concavity and weirdness starts happening.
Why is this happening 😞 ?
Solved! Go to Solution.
There are a couple of settings that I have in my config.pro file that might help:
I don't know what the default for these is, but maybe that's what is causing your troubles. I have both set to 0.00001 in my config.pro file and it works fine, don't know if there is some sort of hard-coded limit built into the software.
If you're using inches for your model, 0.001 is probably not precise enough.
Try defining the curve using these relations. Using this I do not see the inflection in the curve shown above.
/*convert deg to rad
/* define terms used in Y equation
Unfortunately, I still get the same results with your equation. Looks fine until you start zooming in on the curve in Creo.
Same annoying inflection and blunted tip within 10 mm of the front of the cone.
Does it look like that for you too? Do I need to change a setting in Creo or something?
Curvature analysis of 0-10 mm of curve. It does not look like what you have posted. Creo 4 M060 build.
I have used this curve to generate a surface and the reflection curves also do not indicate the inflection of the surface near the nosecone.
Unfortunately, I am using a student version of Creo which does not allow me to open files made with commercial versions.
Just tried to do the curve on a university machine running Creo 3.0, M080 build. Same results - annoying inflection.
It seems I am the common denominator here yet all I'm doing at this point is copy and pasting an equation for a datum curve and I still get weirdness.
This is all pretty weird, but I've seen stuff like this before where the curve and/or surface has in inflection like that but SHOULD be smooth. Perhaps it a rounding/math error, I mean BUG, in Creo?
I wish I could see the model but I'm still on Creo 3... 😞
Here's a theory that seems to prove out when I tried it:
If you go into File->Prepare->Model Properties, and look at the Accuracy setting, I'll bet it's something like "Relative 0.0012" or whatever is the default for your particular site. Because of the relative size of the tip of the nosecone shape you are trying to define, the relative setting will give "chunky" results and not the nice smooth curve you want.
Try setting the Accuracy to something like "Absolute" and a value of 0.00001, then regenerate. The curvature should be more to your liking.
I have confirmed this through testing for this curve (Creo 4). Using default relative accuracy yields the anomalous curve.
Unless one has a compelling reason to do so, relative accuracy should not be used for Creo models. Absolute accuracy should be assigned to models (start parts) in the context of the manufacturing process tolerances that will be used to make them. I have never had a reason to use relative accuracy in Pro/E or Creo in over 25 years on any design project. I have always used absolute accuracy. I recall being told in the 90s by a PTC applications engineer that relative was implemented as default to support faster regeneration of models vs absolute. If anyone has a use case for where relative accuracy would be preferred in a design used to fabricate something I would be interested to hear about it.