Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

How to draw a curve in Creo that is defined by an equation?

samihasamin

New member
So I want to draw a parabola in Creo that is defined by the equation y= (h/(b^2))*x^2

Basically it looks something like this:

Centroid, Area, Moments of Inertia, Polar Moments of Inertia, & Radius of Gyration of a Parabolic Spandrel (Sub-Parabolic Area)

The reason I am asking this is because I need to manufacture a vessel that has curved edges, but I cannot simply give the equation to the fabricator, I have to give him dimensions, and if I draw the curve in Creo it will show the radius of the curve, but I am not sure how to draw a curve that is a function of an equation. If someone knows then please tell me how
 
It should be quite simple with a "curve from equation" where you can write a parametric equation to drive your curve. Check in the datum curve flyout menu
 
You will use the "curve from equation" as zpaolo states. The thing you will have to adapt is you need to write your equation in terms of t. t is an arbitrary parameter which by default goes from 0-1. So for your equation you would need to write it as:
x=t
y=(h/(b^2))*t^2
z=0

I created a parameter "base" and "height" and used in the equation for y.
 
And if you want your x from a different range instead of putting

x=t

where x will go from 0 to 1, just put it like

x=xmin+t*(xmax-xmin)

so x will span the range from xmin to xmax

Paolo
 

Sponsor

Articles From 3DCAD World

Back
Top