Equation Driven Curve is creating a small gap how to get rid of this gap? 2 is over defining the sketch but 1.999 is creating a gap.
pi*10 should be the correct one but it gives over defined sketch. I reduce the number and tried.
Hi maha,
Do it in 2 steps,
First 1 EquationDrivenCurve between 0 and pi, and after another from pi to 2*pi.
After that you can use composite curves to merge both Curves in 1.
Cheers
...not sure,.. but would guess it is a math limitation with closing the loop.. that is, to infinity and beyond.. so, the algorithm includes a stop/gap/limit?).
Hi Maha,
Introducing Pi for the parameter 'T' and talking about trigonometry in radians, means that the equation is evaluated between between 0 and 360 degrees. This is 0 and 2Pi. If you go over 2Pi, the curve will repeat itself, meaning that it would passing from the same point twice. And this is no possible with these type of curves.
My recommendation was to do 2 equation driven curves, first evaluated between 0 and 180 degrees (0-Pi) and second between 180 and 360 (Pi to 2Pi).
So when merging using composite curves, both points will merge because are the same.
Let me know if that works for you.
Cheers.
Hi Maha,
The method is:
Then you can use a single perfectly mathematic close curve for your purposes.
Cheers.
Hi Maha,
If it works better that Paul's answer, I should have the Correct Answer . You don't need to apply any tolerances, you get what you wanted.
Cheers
Is it possible to manipulate the equation that moves the joining points to this apex. Because it is easy have plane if there is a point.
Maha,
From a new 3D Sketch you can recall that curve 'Conver Entities', and then manipulate it as you wish.
Maha Nadarasa please give Marcos Rodríguez or Roland Schwarz the correct answer.... because they are more "correcterist" (+/-0.0001mm?)
This video is also giving same information but using Fit Spline instead of Composite Curve and using negative sign and 0-pi range.
SolidWorks Tutorial: 3D Sketch "Equation Driven Curve" - YouTube
Hi Maha,
Thanks very much.
Well at this stage I believe we should know different options, and choose the one that best fit us, either you want an approximation or keep working with original math equations.
Cheers
Hi Paul,
Fit spline won't result exactly the same curve as original. It's an approximation.
Regards.
Marcos,.. yes,..it's an approximation set with a tolerance on the curve(or entites) selected.
..question,.. assuming the equation is absolute,.. and,..the curve generated is created within the kernel tolerance/limits of Parasolid.....is the equation generated curve (parasolid) also a approximation? "yes/no"
An equation is an equation, pure mathematics, if you draw y=x^2, you will get an exactly math curve, in your screen. So answer is not, not an approximation.
Fit splines are approximations, internally different equations to the one we want.
Cheers.
Thanks Marcos,.. appreciate that!
So,.. maybe it's more of a question of "Absolute/Perfect geometry" in the real world of... science or engineering?
..this Absolute Perfect Curve Driven by a Equation... can only remain perfect,.. by itself, used only within the SolidWorks (a vacuum if you will) or a *.sldprt... that is, if we export that perfect curve,.. it looses the link to the driven equation and perfection and will become a approximation/tolerance per the kernel (or other modeling kernel which imports it).
..now, in the above sweep example,.. when we introduce a circle normal to the end of this "perfect curve",.. and apply a Sweep Feature (in this case.. or any feature)... will the topology be perfect,..and/or, will it be perfect when we export it to X_T or STEP or IGES?
From my perspective,... using 3D tools or working within a realistic tolerance (approximation),.. you may begin with a absolute perfect curve. .but the subsequent feature processes would degrade the original perfect curve.. so.. if the intent is perfection (science).. is would be quickly lost with Solidworks features alone.. and later within manufacturing tolerance processes.
Hi Paul,
Don't take it personal. Your solutions works too, but it's not as good as mine ....
My answer should be the Correctest!!!!
Cheers.
Marcos,.. I don't care about the points (or it being personal), it's not about right/wrong, for me, it's about options which create a design within tolerance... and, I appreciate your input,.. you got 1000 points.
Correctness (+/-?) = what are the tolerance differences between the two curves (Fit Spline and Composite Curve) and finally creating the two child Sweep features or the end result/goal?
Hi Paul,
Thanks for the badge, my first one.
I've learnt new things from these forums. I think this is the most valuable thing. Maha had a problem and we gave 2 different options. His main issue was to understand the parametric equations when use trigonometry and the values of angles in radians.
Your answers weren't clear and resulted confusing. Nobody talked here about kernel, export, machinning, etc... Only you.
Actually I've just extended the answer of:
that was right.
I wrote 'correctest', meaning the most correct in a funny way. I knew was wrong.
Cheers.
..for anyone interested,.. and for reference,.. here are two ways to convert the two halve equations using the Composite Curve and Fit Spline and their compared volumes ... Also.. doing a manual layout, no equations for those who would like to use planes/sketches/curves.
If a gap is tiny it will not make any issue. So far I have no problem with this.
Hi Maha,
Maha Nadarasa wrote:
If a gap is tiny it will not make any issue. So far I have no problem with this.
To me, when I did anything in SolidWorks a gap was a gap and if it was supposed to be there then I considered it as wrong. If I was presented with, or made aware of any gaps, I would correct them because I learnt early on that 9 times out of ten it would come back and bite me later. Now, that's not to say that some of my projects didn't have gaps in them, they probably did, I was just never notified or noticed them. But, if I ever came across one, I corrected it. Just saying.............
Dave.
