Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape, CAD, maker project and design.

First time visiting? Here are some places to start:

  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Parametric Curve Extrude.

ethan_ofondoethan_ofondo Member Posts: 3
Hi, 
I have been using the Parametric Curve Feature Script, but I can't seem to use the curves for anything useful in my model. 
For example, I cannot extrude a plane from the curve, or use multiple curves to define an area to extrude on an existing surface.

Below is a screenshot of what I am trying to do. I have two equation-driven curves that have been defined in the x-y plane, where the z coordinate matches that of the extruded surface that is visible. I am now trying to remove material between the two curves. Any suggestions?




 

Comments

  • ilya_baranilya_baran Onshape Employees, Developers Posts: 829
    The simplest thing you can do interactively is to define a sketch and project the curves onto the sketch using the "use" button (in sketch, icon looks like a cube).  Once they're sketch curves, you can use them for bounding sketch regions or for extrusions.  Otherwise, you can use the curves for things like sweeps and lofts and for constructing planes.
    Ilya Baran \ Director of FeatureScript \ Onshape Inc
  • ethan_ofondoethan_ofondo Member Posts: 3
    Thanks @ilya_baran. The "use" tool solved my problem. 
  • mike_evermanmike_everman Member Posts: 7 PRO
    Trying as well to use the parametric curve fs, and my first cut at formatting an equation is not valid, and having a lot of trouble finding help files on the subject.
    I'm trying to do the cartesian equation for a cycloid curve.  I originally had two parameters, but now am typing in the Radius of the generating circle (248mm) and keeping it to one param.

    248mm*(acos(1-#y/248mm))/deg*pi/180-sqrt(2*248mm*#y-#y^2)
    I feel like such a noob.
    Here is the equation:

    Anyone feel like attaching the electrodes of knowledge on me?

    Mike Everman
  • mike_evermanmike_everman Member Posts: 7 PRO
    Ah, found the instructions in the feature script.  Never mind.
  • mike_evermanmike_everman Member Posts: 7 PRO
    Hi @ilya_baran , can you possibly help me code this cartesian cycloid curve?  R is the radius of the generating circle.  I can't seem to get the parametric curve fs to do it, and fear I'm just not understanding the rules of syntax.

    Best regards,
    Mike
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,022
    edited August 10
    Hi @mike_everman

    I think the trouble you're experiencing is probably that you need an independent variable that represents the parameterization of the curve.

    In this case lets pick an arbitrary variable "t", and say that "t" moves from 0 to 2R (it seems that this is the domain of this function).

    Then we need to define x, y, and z in terms of "t".
    z is easy.  It seems like you're trying to plot this in 2d, so we can just say that z is 0.
    Since y appears to be the driving factor in your equation, we can say that y is t.
    Now, we can set x to R*acos(1-t/R) - sqrt(2 * R * y - y^2).

    Due to the fact that t should be a unitless parameter, I will divide t by some arbitrary unit (here I am choosing inch) for the definition of the range of t, and multiply by the same arbitrary unit everywhere I decide to use t.  So the parameters will actually look like:
    t is 0 to (2R / inch)
    X is R*acos(1- (t * inch)/R) - sqrt(2*R*(t*inch) - (t*inch)^2)
    in Onshape syntax: #R*(acos(1-(#t*inch)/#R)/radian) - sqrt(2*#R*(#t*inch)-(#t*inch)^2)
    Y is t * inch

    Here it is an a part studio:
    https://cad.onshape.com/documents/223a8b97a2f7f469664b4bd5/w/d48f2b3f6a952d52981f6990/e/ff814e7f9f5409604eceff8d

    Hopefully this curve looks similar to what you were looking for?

    Jake Rosenfeld - Modeling Team
  • mike_evermanmike_everman Member Posts: 7 PRO
    That's the curve!  Thank you Jake!  I was certainly not grokking the units and where they go.
  • mike_evermanmike_everman Member Posts: 7 PRO
    @Jake_Rosenfeld ; one more thing any way I can improve the tesselation on the display of this curve?  Though this partial curve has 1,000 points, I see polygonal facets of 5mm!

  • kevin_o_toole_1kevin_o_toole_1 Onshape Employees, Developers Posts: 396
    edited August 10
    Currently you can only adjust the tessellation quality of parts and surfaces in Onshape (which can be done in the "Edit appearance..." dialog). Adjusting the appearance/quality of curves sounds like a great improvement request :) Until then, you could try sweeping an edge along the curve and refining the tessellation quality of the resulting surface.
Sign In or Register to comment.