How can i create sinusoidal pattern around a circle by using equation driven curve?Is there any other method to draw the sinusoidal patterned geometry?
Equation driven curve is probably the way to go on this. Your general equation of radius as a function of theta would be...
r(ϴ) = r₀ + δ*sin(ω*ϴ)
SOLIDWORKS isn't going to take that equation directly so you would have to convert it using the parametric forms below:
x(ϴ) = r*cos(ϴ)
y(ϴ) = r*sin(ϴ)
With the r(ϴ) substituted in for r you get these:
x(ϴ) = (r₀ + δ*sin(ω*ϴ))*cos(ϴ)
y(ϴ) = (r₀ + δ*sin(ω*ϴ))*sin(ϴ)
...which goes right into the definition of an equation driven curve. If we use these dummy values:
ϴ=t, for the range t=0 to t= 2π
...you get this:
Hello Ryan sir,
Thank you for replying to my question.I have implemented it in the same way as you did.But, the is that the sinusoidal patterns endpoint is not coinciding with the starting point(i.e there is a gap in between these two point at t=0 and t=2*3.14).I am attaching you the file. How to solve this?
Awaiting for your Response..
I guess thats because of the approximation of PI. How about using the equation to create just one single waveform, make it into a feature and circular pattern it?
I let the equation curve go slightly past the 36 degree point and extruded the region
then convert entities
edit: on second thought not so ideal maybe
Hi Rob Edwards,
Thank you for solving the problem.
I am trying to draw the pattern by taking the equation itself.Can it be possible ?
I think the reason why you cannot do this is AFAIK Solidworks will not allow you to form a closed loop from an equation curve.
I have a couple of bits of good news though
You can use PI directly in the equation
But with a value for t2 of 2 * PI this happens
so going back to my previous post, this works better using the constant PI
Here I used a circular pattern of a planar surface, followed by a Fit Spline
If you don't want to do that, there have been many posts on the forum about sketch patterns being a bit dodgy, but you can try
and it kind of works...
but I couldn't get it to constrain
I have to draw this geometry in 2D form. In solid works if i am taking the surface then extrude option is available, i have to take the surface only.How to do that?I am attaching an image.I have to draw a sinusoidal pattern circle, after that i have to draw a circle which acts as a domain and i have to take the surface between the outer circle and pattern as shown in the figure.In Ansys surface from sketches option is available by taking that option one can able to take surface from sketch.But in solid work i didn't find surface from sketches option.how to do it?
You need to use the surface tools. Either copy the face of a 3d body using offset surface..
Or make a planar surface and knit
The surfacing tab may not be active on your command manager if you dont see it just right click a tab and activate it
Hello Sir ,
Thank you for quick response.
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